树莓派出版社

Raspberry Pi Press

store.rpipress.cc

store.rpipress.cc

Raspberry Pi Press 是您进行计算机、游戏和动手实践的必备书架。我们是 Raspberry Pi Ltd. 的出版品牌。从组装 PC 到制作机箱，我们丰富的书籍和杂志将帮助您发现兴趣所在，学习新技能，并创造出令人惊叹的作品。

Raspberry Pi Press is your essential bookshelf for computing, gaming, and hands-on making. We are the publishing imprint of Raspberry Pi Ltd. From building a PC to building a cabinet, discover your passion, learn new skills, and make awesome stuff with our extensive range of books and magazines.

MagPi

The MagPi

magpi.raspberrypi.com

magpi.raspberrypi.com

MagPi是树莓派官方杂志。它面向树莓派社区，内容涵盖树莓派主题项目、计算机和电子教程、操作指南以及最新的社区新闻和活动。

The MagPi is the official Raspberry Pi magazine. Written for the Raspberry Pi community, it is packed with Pi-themed projects, computing and electronics tutorials, how-to guides, and the latest community news and events.

一大袋插座

A sackload of sockets

您将在原理图中再添加三个 20 针连接器。再次单击“添加符号”工具图标，但请注意，随着库列表区域的填充，顶部会出现一个“最近使用”区域，其中列出了 20 针连接器（您可能需要滚动库列表区域才能看到它）。单击此列表，然后单击“确定”，再将下一个连接器添加到原理图中。重复此操作，直到添加四个连接器。

You are going to place three more of 20 pin connectors into the schematic. Click the Add a Symbol tool icon again, but notice that, as the library list area populates, you now have a Recently Used area at the top with the 20-pin connector listed underneath (you may need to scroll the library list area to the top to see this). Click this listing and then OK, then place the next connector in the schematic. Repeat this until you have placed four of the connectors.

接下来，使用M（移动）快捷键移动连接器，使两对连接器并排排列。其中一对连接器位于 Pico 的左侧，一个连接器是 Pico 引脚的插孔，另一个连接器是用于连接其他硬件的插孔。另一对连接器位于右侧，情况相同。

Next, use the M (Move) hotkey to move the connectors so that there are two pairs of connectors next to each other. One pair of headers corresponds to the left side of the Pico with one header being the holes for the Pico’s pins and one header being holes to attach additional hardware. The other pair is the same thing but on the right-hand side.

使用快捷键（例如M）时，只需将光标悬停在符号上，然后按下快捷键即可——无需先选中符号。快捷键可以作用于整个符号及其各个部分。要选中整个连接器，最简单的方法是将光标放在组件内部的空白区域，然后按下快捷键。可能需要尝试几次才能熟练掌握。如果难以将光标放在正确的位置，可以尝试稍微放大视图。

When using hot keys like M, place the cursor over the symbol and then press the key — there’s no need to highlight the symbol first. The hot key can work on the complete symbol as well as individual parts of it. The easiest way of grabbing the whole connector is to place your cursor in a bit of blank space inside the component, then press the key. It might take a few attempts to get the hang of it. If you find it hard to get your cursor in the right place, try zooming in a little.

现在你应该有两对连接器，为了方便连接电线，你需要将电线连接到连接器内侧的小圆圈上——这些圆圈就是你要连接电线的地方，而且电线不要穿过圆圈，这样看起来会更整齐。你可以使用X（水平镜像）快捷键来完成这个操作。你只需要对每对连接器中最右边的那个进行此操作即可。

You should now have two pairs of connectors, but to make it easier to connect the wires, you’ll want the little circles on the inside of the pair — these are the bits you’ll connect the wires to and it’s a bit tidier if the wires don’t go across the symbol. You can do this using the X (Mirror Horizontally) hot key. You’ll only need to do this for the rightmost connector in each pair.

虽然这次你不需要用到它，但R（旋转）快捷键通常也有助于将零件调整到合适的位置。

Although you don’t need it this time, the R (Rotate) hotkey is often also useful for getting your parts in a useful place.

使用“添加导线”（单击工具箱中的图标或按W键）工具，您可以单击其中一个连接器引脚圆圈，然后绘制一条导线连接到对面的连接器引脚（图 1-5）。如果操作失误，可以使用Ctrl+Z撤销上一步操作；或者，要在绘制过程中取消导线，可以右键单击并从下拉菜单中选择“取消” 。

Using the Add a Wire (click on the icon in the toolbox or press W) tool, you can click on one of the connector pin circles and then draw a connector wire line across to the opposite connector pin (Figure 1-5). If you make a mistake, you can use CTRL+Z to undo the last action — or, to cancel the wire mid-draw, you can right-click and select Cancel from the drop-down menu.

继续连接每对连接器上相对的引脚，直到所有连接器都连接在一起。请注意，每个连接器符号都包含一些文本说明。建议您编辑这些说明，使其更易于理解和记忆。选中其中一个连接器符号（使用选择工具框选整个符号），将光标悬停在该符号上，然后按E键。

Continue to wire between each of the opposite pins on each connector pairs until they are all connected together. Notice that each of the connector symbols have a couple of text references as part of them. It can be good practice to edit these so that they are useful and help you keep track of what things are. Select the whole of one of the connector symbols (use the selection tool to draw a box over the entire symbol), put the cursor over the symbol, and then press E.

现在您应该会看到“符号属性”对话框（图 1-6）。您可以编辑“参考”（如果需要）和“值”文本条目。您应该为每个连接器指定一个描述性值，例如“左侧 Pico”。这在 PCB 编辑器中布局 PCB 时非常有用，因为它可以确保您能够正确识别各种连接器。

You should now see a Symbol Properties dialogue box (Figure 1-6). You can now edit the Reference (if required) and the Value text entries. You should give each connector a descriptive Value such as Left Pico. This is useful when you lay out the PCB in the PCB Editor, as it ensures you can identify the various connectors correctly.

为了完成原理图，添加一个电阻和一个LED，并将它们连接到Pico的38号引脚（GND）和36号引脚（3.3V（输出））。这两个引脚分别是右侧连接器上的第三个和第五个引脚。使用之前选择符号的相同方法，搜索“R”表示电阻，搜索“ LED”表示LED 。如图1-7所示，添加导线连接电路。如果需要，可以使用快捷键“R”旋转符号。

To finish the schematic, add a resistor and an LED and connect them to pins 38 (GND) and 36 (3V3 (OUT)) on Pico. These pins are the third pin and fifth pin down on the right-hand connector. Use the same techniques you used earlier to choose a symbol, searching R for a resistor and LED for an LED symbol. Add wires to connect the circuit, as shown in Figure 1-7. Use the R hotkey to rotate symbols if needed.

已开启

Switched on

接下来，添加一个开关符号，将其连接成 Pico 的复位按钮。

Next, add a switch symbol which you will wire in as a reset button for the Pico.

添加复位按钮很好地体现了 KiCad 与其他一些电子设计自动化 (EDA) 工具的不同之处。在某些 EDA 工具中，您在原理图级别选择的符号会精确定义 PCB 上电子元件的硬件封装。

Adding a reset button is a good example of a way that KiCad works differently to some other Electronic Design Automation (EDA) tools. In some EDA tools, the symbol you choose at the schematic level defines exactly the hardware package of the electronic component that will be on the PCB.

在其他EDA工具中，您不会放置通用的电阻符号，而是放置与特定电阻关联的电阻符号，例如一个6mm长、1/4瓦的水平放置的碳膜电阻。这意味着，如果您想更改PCB上的元件，则必须修改原理图。在KiCad中，原理图符号仅分配一个 封装——这就是为什么您要放置一个单刀单掷开关（SPST）的符号，但实际元件可以是任何SPST开关或任何按钮封装。在本例中，您将选择某种瞬时按钮作为复位按钮。这种工作方式意味着，如果您发现需要用不同类型的元件替换某个元件（例如，如果您找不到库存元件），您只需更改与符号关联的封装，而无需编辑原理图。它还能使原理图简洁易读，这对于共享设计至关重要。

In other EDA tools, you wouldn’t place a generic resistor symbol, you would place a resistor symbol linked to a specific resistor, say a 6mm long 1/4-watt carbon resistor placed horizontally. This would mean that, if you wanted to change the component on the PCB, you have to change the schematic. In KiCad, the schematic symbol is only assigned a footprint — this is why you are going to place a symbol for a single-pole single-throw switch (SPST), but the actual component can be any SPST switch or any button package. In this case, you’ll choose some type of momentary push-button for the reset. This way of working means that if you find you need to replace a component with a different type (for example, if you can’t find a component in stock), you simply change the footprint associated with the symbol and don’t have to edit your schematic. It also makes the schematics concise and readable, which is important if you want to share your design.

要添加开关，请在“选择符号”对话框中搜索sw_spst，即可直接找到单刀单掷开关，然后按照图 1-8所示连接导线。最后，添加四个连接器作为电路板上的原型区域；搜索conn_01x04即可直接找到该符号。现在，您的原理图应该如图 1-9所示。

To add the switch, search the Choose a Symbol dialogue with sw_spst to take you directly to the single-pole single-throw switch and again connect wires, as shown in Figure 1-8. Finally, add four connectors to act as prototyping areas on the board; search for conn_01x04 to take you directly to this symbol. You should now have a schematic that looks like Figure 1-9.

让我们为每个原理图符号设置关联的封装。转到“工具”>“分配封装”。此时将出现“分配封装”对话框（图 1-10），左侧是封装库列表，中间部分是项目中原理图符号的列表，右侧是筛选后的封装结果。窗口顶部有三个名为“封装过滤器”的图标，稍后您会看到，选择第二个图标（按引脚数筛选）会很有帮助。随着您逐渐熟悉元件筛选，您可能会发现自己更喜欢使用这些筛选工具的不同组合。

Let’s set up the associated footprints for each schematic symbol. Go to Tools > Assign Footprints. The Assign Footprints dialogue (Figure 1-10) appears with a list of footprint libraries down the left-hand side, a centre section with a list of schematic symbols in the project, and a right-hand column of filtered footprint results. There are three icons at the top of the window called Footprint Filters and, as you’ll see in a moment, it’s helpful to select the second of these (Filter by pin count). As you get used to component filtering, you might find you prefer to use different combinations of these filtering tools.

在中心区域选中一个 20 针连接器元件。你需要找到一个引脚数相同且每个引脚都对应一个通孔焊盘的封装。由于 Raspberry Pi Pico 的引脚间距为常见的 2.54mm，因此你还需要确保封装的间距与之相同。右侧应该会显示一个筛选列表——该列表应仅包含与 20 针连接器符号对应的元件。从连接器封装库中选择 Connector_PinSocket_2.54mm :Pinsocket_1x20_P2.54mm_vertical。单击一次以在列表中选中该元件，然后使用“在封装查看器中查看所选封装”工具图标（从左数第三个图标）打开一个窗口，显示 PCB 封装布局设计，以检查其是否正确。 双击选中的封装，将其与中心列表中选定的原理图符号关联起来。继续操作，将相同的封装添加到所有四个连接器符号列表中（稍后我们将讨论为什么这样做并不完全正确，但对于这个入门项目来说没问题）。单击“应用、保存原理图并继续”按钮。

Highlight one of the 20-pin connector components in the centre section. You need to find a footprint that has the same number of pins and has a footprint of a through-hole pad for each pin. As the Raspberry Pi Pico pins are spaced at the common 2.54mm pitch between each pin, you also need to make sure the footprint is spaced similarly. You should have a filtered list on the right-hand side — it should be filtered to only contain items that would attach to the 20-pin connector symbol. Choose Connector_PinSocket_2.54mm:Pinsocket_1x20_P2.54mm_vertical from the connector footprint library. Click once on the item to highlight it in the list, then use the View the selected footprint in the footprint viewer tool icon (third icon from the left) to open a window showing the PCB footprint layout design to check if it looks correct. Double-click the highlighted footprint to associate it with the selected schematic symbol in the central list. Continue and add the same footprint to all four connector symbol listings (we’ll discuss later why that isn’t totally correct, but it’s fine for this starter project). Click the Apply, save schematic and continue button.

您还需要添加 LED、电阻和按钮的表面贴装元件；请选择易于手工焊接的 SMD 封装尺寸和焊盘。LED 选择 LED_SMD :LED_0805_2012Metric焊盘；电阻选择Resistor_SMD:R_0805_2012Metric 焊盘；开关选择Button_Switch_SMD:SW_SPST_B3SL-1002P元件。对于分离式 4 针连接器，每个连接器选择Connector_PinSocket_2.54mm:PinSocket_1x04_P2.54mm_Vertical 焊盘 。分配完所有焊盘后，单击“应用”，保存原理图并继续，然后单击“确定”。

You’ll also need to add surface-mount components for the LED, resistor, and the button; you’ll choose SMD package sizes and footprints that are easy to hand-solder. For the LED, choose the LED_SMD:LED_0805_2012Metric footprint; for the resistor, the Resistor_SMD:R_0805_2012Metric; and for the switch, a Button_Switch_SMD:SW_SPST_B3SL-1002P component. For the detached 4-pin connectors, select Connector_PinSocket_2.54mm:PinSocket_1x04_P2.54mm_Vertical for each connector. With all those footprints assigned, click Apply, save schematic and continue, then click OK.

在下一章中，您将把元件封装列表导入 PCB 编辑器，并实际布局电路板设计，使其准备好进行制造。

In the next chapter, you will import the list of component footprints into the PCB Editor and physically lay out the board design to get it ready for fabrication.

除了脚印什么都不要留下

Leave only footprints

接下来，您可以将相对焊盘上的焊盘连接起来（图 2-6）。为此，请选择“布线 (X)”图标，然后单击一个焊盘的中心，并将走线拖动到相对焊盘的中心。走线应为红色，表示它位于顶层铜箔上。例如，如果您移动到​​B.Cu (PgDn)层，则底层铜箔上的走线默认颜色为蓝色。继续连接所有焊盘，您会发现连接过程中杂乱的线路会消失。

Next, you can wire the pads on the opposite footprints together (Figure 2-6). To do this, select the Route Tracks (X) icon, then click the centre of a pad and drag the track over to the centre of the opposite pad. The track should be red, indicating that it’s on the top copper layer. If you, for example, were to move to the B.Cu (PgDn) layer, the default colour for tracks on the lower copper layer is blue. Continue and connect all pads together, noticing that the rat’s nest lines disappear as you do so.

参考 Pico 技术图纸，现在是定义电路板形状和边缘的好时机。为此，您可以使用最上方的下拉菜单，从F.Cu（PgUp）图层切换到Edge.Cuts图层。在该图层上，您将使用“绘制矩形”工具为电路板创建切口形状。但在选择此工具之前，请将网格间距切换到更合适的值。选择 1mm 网格间距，然后单击矩形工具。在 PCB 编辑器页面中单击任意位置并拖动一个矩形（图 2-7）。它不必覆盖其他元件，因为您将在下一步中移动它。

Referring to the Pico technical drawing, it’s a good time to define the shape and edges of the board. To do this, you can use the uppermost drop-down menu to move from the F.Cu (PgUp) layer to the Edge.Cuts layer. On this layer, you will use the Draw a Rectangle tool to create a cutout shape for the board. But before you select this tool, switch the grid to a more useful spacing. Select the 1mm grid spacing, then click the rectangle tool. Click anywhere in the PCB Editor page and drag a rectangle (Figure 2-7). It doesn’t have to be over the other components because you’ll move it in the next step.

矩形应自动吸附到网格上，然后将其拖动，直到标签显示其宽度为 21 毫米，高度为 51 毫米。再次单击以创建矩形。返回“选择项目”工具，现在选中矩形并按M键将其移动到所需位置。从 Pico 技术图纸中可以看到，Pico 的外边缘距离密码键盘中心 1.61 毫米。为了精确定位，应将网格间距缩小到最小值，并使用以下方法测量页面上的距离。

The rectangle should snap to the grid, and you should drag it out until the labels tell you that it’s 21mm wide by 51mm high. Click one more time to create the rectangle. Moving back to the Select Items (s) tool, you should now select the rectangle and press the M key to move it into position. Notice from the Pico technical drawing that the outside edge of the Pico sits 1.61mm from the centre of the pin pad position. To position this accurately, you should reduce the grid spacing to the smallest listed and use the following technique to measure distances on the page.

在 PCB 编辑器中，如果您按下空格键，可能会注意到标记为dx、dy和dist的值被设置为零。这非常有用，因为您可以将指针放在某个点上，例如右上角焊盘的中心，按下空格键创建一个零点或基准点，然后将指针移动到（在本例中）边缘切割矩形。之后，您可以使用dx和dy值来帮助您精确定位该矩形或任何其他需要定位的元素。

If you press the space bar at any time when in the PCB Editor, you might notice that values labelled dx, dy, and dist are set to zero. This is very useful as you can place your pointer at a point, say the centre of the top rightmost pad, press the SPACE bar to create a zero or datum point, and then move the pointer to, in this case, the edge cut rectangle. You can then use the dx and dy values to help you position this, or anything you need to, accurately.

正确定位电路板边缘矩形后，即可在 3D 查看器中初步查看电路板。要查看 PCB，请点击“视图”>“3D 查看器”。您将看到电路板，但会注意到所有排针插座的 3D 模型都放置在相应的孔位中。实际上，您只需要在电路板背面安装外侧几排的排针，内侧几排则保持空置，或者安装排针。您可以编辑电路板和元件封装以反映这一点，但在这个简单的示例中，您可以点击“切换通孔元件的3D 模型(T)”图标来关闭这些模型（图 2-8）。在后续章节中，我们将探讨如何使用正确的 3D 模型，以及如何添加自定义 3D 模型。

Once you have positioned the board edge rectangle correctly, you can get a first glimpse of the board in the 3D Viewer. To view the PCB, click View > 3D Viewer. You’ll see the board, but you’ll notice that all the 3D models of the header sockets are all placed into the rows of holes. In reality, you would only want headers on the outer rows installed on the back of the board, with the inner rows left unpopulated, or possibly populated with header pins. You could edit the board and the component footprints to reflect this, but for this simple example, you can click the Toggle 3D Models for Through Hole type Components (T) icon to turn off the models (Figure 2-8). In future chapters, we’ll explore not only using correct 3D models but will look at how you can add custom 3D models too.

保持距离

Keep your distance

现在您可以继续排列和连接剩余的元件。为了使元件排列整齐，您需要切换到 0.635mm 的网格，并且可能需要使用R快捷键旋转开关。您会发现需要稍微重叠一些封装。这样做时，您需要了解封装的每个部分所显示的内容。

You can now continue to arrange and wire the remaining components. In order to fit the components, you’ll need to switch to the 0.635mm grid, and you may need to rotate the switch using the R hotkey. You’ll find that you need to overlap some of the footprints slightly. When doing this, you need to understand what each part of the footprint is showing.

紫色方框标示了元件的最大尺寸。正常情况下，这些尺寸不应重叠。但是，对于排针来说，您实际上并不会添加物理排针（您只是利用这个封装在正确的位置提供一系列通孔）。因此，这些紫色矩形可以略微重叠。浅黄色线条是丝印——也就是印刷在PCB上的图案。同样，对于这块电路板，只要不影响实际元件，这些图案可以略微重叠。随着电路板上实际元件数量的增加，您需要更加注意避免元件之间相互干扰。

The purple box around it shows the maximum size of the component. In normal usage, these shouldn’t overlap. However, in the case of the headers, you’re not actually going to add physical headers (you’re just using this footprint to give you a series of through holes in the right place). Therefore, it’s fine to overlap these purple rectangles slightly. The pale yellow lines are silkscreen — basically, graphics that are printed onto the PCB. Again, for this board, these can overlap slightly provided it won’t interfere with actual components. As you move onto boards with more actual parts on them, you’ll need to be much more careful about things not getting in the way of each other.

对于 LED 和按钮，您需要将走线直接连接到 Pico 的引脚。您会发现必须将走线穿过其他元件。每条走线都必须避开其他元件的焊盘和通孔，但只要避开这些，就可以穿过封装。右键单击即可为导线添加一个弯曲点。

For the LED and the button, you need to wire traces directly to the pin connections to the Pico. You’ll find that you must weave the traces through other components. Each trace has to avoid pads and through holes of other components but can travel through the footprint as long as it misses these. A single right-click adds a bend point to a wire.

您可能需要将组件旋转 180 度，才能使连接线从正确的方向引出。您也可能会发现，减小网格尺寸可以更精确地放置走线，从而获得更好的效果。

You might find that you need to rotate a component through 180 degrees to make the connections come out of the right sides. You might also find that it works better if you decrease the grid size to allow you to place the tracks more precisely.

你的电路板布局比较拥挤，没有太多空间放置文字。你之前用来标记各个接头的标签在PCB布局完成后就不再需要了，所以你可以直接删除它们（点击文字并按删除键）。

You have quite a crowded board, and there’s not much space for text. The labels that you used to remind yourself which header is which are no longer needed once you’ve laid out the PCB, so you can simple delete these (click in the text and press the DELETE key).

最后，如何才能制作出这样的电路板呢？方法有很多——本书将逐一介绍。世界各地有很多公司提供电路板制造和组装服务。

Finally, how do you get this board made? Well, there are lots of options — we will look at many of them throughout this book. There are many services available from companies all over the world to manufacture and even assemble your boards.

这些服务在上传所需信息和文件方面可能需要不同的方法。通常，您需要导出PCB每一层的Gerber文件，以及显示孔的位置和尺寸的钻孔文件。一些公司可能对他们能够生产的孔径和电路板的公差有限制。我们将在后续章节中进一步探讨这一点，但如果您希望获得高质量的电路板，请将以.kicad_pcb结尾的文件上传到OSHPark网站（oshpark.com）。该网站和服务非常出色。它会在浏览器中生成您电路板的多个渲染图，您可以检查这些渲染图是否正确，然后再将PCB添加到购物车进行生产。几周之内——通常更短——您就能收到“完美的紫色PCB”。

These services may need different approaches in terms of what information and files you need to upload to get the job done. Often you’ll need to export Gerber files for each layer of the PCB, and also export drill files which show the position and size of holes. Some companies might have limitations on what size holes they can produce and what tolerance they can produce the board too. We’ll explore this further in future chapters, but if you want to get this board fabricated to an excellent standard, upload the file that ends with .kicad_pcb to the OSHPark website (oshpark.com). The website and service are brilliant. In-browser, it creates numerous renders of your board, which you can then inspect and check to see if they are correct before adding the PCB to your cart to be manufactured. In a few weeks — often less — you’ll have ‘Perfect Purple PCBs’ through your door.

利用库

Leveraging libraries

打开 KiCad，在主页面中，点击“首选项”下拉菜单，然后选择“管理符号库”选项。这将打开一个包含两个选项卡的窗口：“全局库”选项卡和“项目特定”选项卡（图 3-2）。确保您位于“全局库”选项卡中，找到并点击小文件夹图标。导航到您下载的文件夹并打开它，找到名为KiCad_stamp_lib的文件夹。打开此文件夹，选择RP2040_Stamp.kicad.sym 文件，然后点击“打开”。

Open KiCad and, in the main page, click the Preferences drop-down menu and then select the Manage Symbol Libraries option. This should open a window with two tabs: the Global Libraries tab and the Project Specific tab, (Figure 3-2). Ensuring you are on the Global Libraries tab, find and click the small folder icon. Navigate to the folder you downloaded and open it to find a folder called KiCad_stamp_lib. Open this folder and select RP2040_Stamp.kicad.sym and then click Open.

现在您应该能在“全局库”选项卡底部看到一个名为RP2040_Stamp的新库。如果您创建一个新项目并打开原理图编辑器，现在可以使用“添加符号”工具将 Solder Party Stamp 符号添加到原理图中。您可以通过搜索RP2040并确保从RP2040_Stamp 库中选择符号（而不是默认的RP2040符号）来完成此操作；或者，您也可以向下滚动库列表，选择RP2040_Stamp，然后选择RP2040_Stamp符号。

You should now see a new library listed at the bottom of the Global Libraries tab called RP2040_Stamp. If you create a new project and open the Schematic Editor, you can now use the Add a Symbol tool to place a Solder Party Stamp symbol into the schematic. You can do this by searching for RP2040 and making sure you select the symbol from the RP2040_Stamp library (rather than the stock RP2040 symbol) or by scrolling down the list of libraries, selecting RP2040_Stamp, and then selecting the RP2040_Stamp symbol.

添加封装库的操作步骤类似。同样，在 KiCad 主界面，点击“首选项”，然后点击“管理封装库”。在“全局库”选项卡中，点击小文件夹图标（图 3-3）。找到您下载的文件夹，找到KiCad_stamp_lib文件夹——再次打开该文件夹，但这次选择RP2040_Stamp.pretty文件夹，然后点击“打开”。您应该会看到里面有三个文件，但无需选择任何特定文件——只需再次点击“打开”即可。现在，回到“全局库”选项卡，您应该可以向下滚动并看到RP2040_Stamp库条目。您可以通过将正确的封装与您在原理图编辑器中放置的RP2040_Stamp符号关联起来来检查操作是否成功，然后您可以打开该元件并将其导入到 PCB 编辑器中。如果您需要回顾一下如何执行这些操作，我们在前面的章节中已经介绍过。

It’s a similar experience to add a footprint library. Again, in the KiCad landing page, click Preferences and then Manage Footprint Libraries. Again, on the Global Libraries tab, click the small folder icon (Figure 3-3). Navigate to the folder you downloaded and find KiCad_stamp_lib — open that folder once more but, this time, select the RP2040_Stamp.pretty folder and click Open. You should see three files inside, but you don’t need to select any particular one — just click Open again. Now, back on the Global Libraries tab, you should be able to scroll down and see an RP2040_Stamp library entry. You can check that this has all worked by associating the correct stamp footprint to the RP2040_Stamp symbol you placed in the Schematic Editor, and then you can open and import the part into the PCB Editor. If you need a reminder on how to do those tasks, we covered them in the previous chapters.

使用 BMP280 模块，您可以学习如何创建原理图符号和封装。为此，您需要创建自己的库来存放这些元件以及将来可能添加的其他元件。我们先从自定义原理图符号开始。在原理图编辑器中，单击“创建、删除和编辑符号”工具按钮。这将打开原理图符号编辑器。

Using the BMP280 module gives you an opportunity to learn how to make both a schematic symbol and a footprint. To do this you will create your own libraries to contain these parts, and others in the future. Let’s begin with a custom schematic symbol. In the Schematic Editor, click the Create, delete and edit symbols tool button. This opens the Schematic Symbol Editor.

在新窗口中，单击“文件”，然后从下拉菜单中选择“新建库” 。此时应该会看到一个名为“添加到库表”的小对话框。在此对话框中，您可以选择将新库添加到“全局”表。这意味着 KiCad 中的任何项目都可以访问此库；或者，如果您选择“项目”，则只有此 KiCad 项目可以访问该库。由于 BMP280 是您可能在其他项目中使用的对象，请确保选中“全局”，然后单击“确定”。接下来，系统会提示您为库命名——您可以随意命名，但请确保保留文件名中的“.kicad_sym”部分，然后单击“保存”。

In this new window, click File and then select New Library from the drop-down menu. You should now see a small dialogue box called Add To Library Table. In this box, you can select to add your new library to the Global table. This means any project in KiCad can access this library; alternatively, if you select Project, only this KiCad project can access that library. As the BMP280 is something you might use in other projects, make sure Global is highlighted and then click OK. You’ll now be asked to give your library a name — it can be anything you want, so name it, making sure to leave the .kicad_sym part of the file name intact, and click Save.

现在您应该能在符号编辑器窗口左侧看到高亮显示的符号库名称。这意味着该符号库已激活，因此当您选择创建新符号时，它将被存储在该符号库中。

You should now see your new symbol library name highlighted on the left-hand side of the Symbol Editor window. This means that this is the active library, so that when you select to create a new symbol, it will be stored in this library.

点击“文件” ，然后从下拉菜单中选择“新建符号” 。此时应该会弹出“新建符号”对话框。给符号命名，该名称将出现在库列表中——最好选择一个能够反映元件特性的名称，例如：pi_bmp280。点击“确定”后，符号编辑器窗口中应该会出现一个“U”符号，并且该符号的名称会出现在屏幕左侧列表的活动库中。名称旁边会有一个星号（*），表示该符号尚未保存。

Click File and select New Symbol from the drop-down menu. You should see a New Symbol dialogue appear. Give your symbol a name that will be used in the library list — make it a useful name that reflects the part: pi_bmp280. Clicking OK, you should now see that a U has appeared in the Symbol Editor window and that the name of the symbol now appears in the active library in the list on the left-hand side of the screen. The name will have a * next to it, indicating that the symbol has not been saved.

符号编辑器中有一些熟悉的控件，例如F1和F2键，用于放大和缩小。稍微缩小一下，给自己留出一些空间，就可以开始添加引脚了。

In the Symbol Editor there are some familiar controls, such as the F1 and F2 to zoom in and out. Zoom out a little to give yourself some room and you can get started by adding some pins.

点击“添加引脚”工具图标。在对话框中，您可以为引脚命名、编号、设置电气类型，并根据需要更改其他设置。对于第一个引脚，将其命名为“1” 2-6V_in，分配引脚编号“ 2 1”，并将电气类型设置为“电源输入”。继续添加引脚 2、3、4 和 5，并按照图 3-4所示进行标记。放置引脚时，请注意您可以使用通用快捷键M（移动）和R （旋转），类似于原理图或 PCB 编辑器中的操作。创建所有引脚后，使用“添加文本项”工具添加文本标签。这样，在查看原理图时，您可以快速识别符号。

Click the Add a pin tool icon. In the dialogue, you can name the pin, give it a number, set its Electrical type, and change other settings if needed. For the first pin, name it 2-6V_in, assign it pin number 1, and set the electrical type to Power input. Continue to add pins 2, 3, 4, and 5, labelling them as you can see in Figure 3-4. As you place pins, notice that you can use the generic hot keys M for move and R for rotate, similar to the Schematic or PCB Editors. Once you have all your pins created, add a text label using the Add a text item tool. This lets you identify the symbol quickly when looking at a schematic.

最后，在原理图符号周围绘制一个边界框，使所有元素整齐地组合在一起。单击“添加矩形”工具，在设计上绘制一个矩形。单击屏幕左上角的“保存”图标，然后关闭符号编辑器窗口。现在，您可以进入原理图编辑器，使用“添加符号”工具查找并添加您的第一个自定义符号。

Finally, draw a bounding box around the schematic symbol so that everything is neatly grouped together. Click the Add a rectangle tool and draw a rectangle over your design. Click the Save icon in the top-left corner of the screen, and then close the Symbol Editor window. You can now go into the Schematic Editor and use the Add a symbol tool to find and add your first custom symbol.

接下来，为 Pimoroni BMP280 模块创建一个新的封装库和封装。首先，打开封装编辑器（图 3-5）。您可以从 KiCad 主项目窗口或PCB 编辑器中的“创建、删除和编辑封装”工具图标打开它。与符号编辑器类似，打开封装编辑器后，首先单击“文件”，然后从下拉菜单中选择“新建库” 。选择将新库添加到“全局”或“项目”表——选择“全局”并为您的库命名。新库出现在列表中后，选中它，然后单击“文件”并选择“新建封装”。此时将出现一个对话框，您可以在其中为新封装命名：Pim_BMP280_Module。

Next, make a new footprint library and footprint for the Pimoroni BMP280 module. To begin, open the Footprint Editor (Figure 3-5). This is available from either the main KiCad project window or from the Create, delete and edit footprints tool icon in the PCB Editor. Similar to the Symbol Editor, once you have the Footprint Editor open, the first thing to do is to click File and then select New Library from the drop-down menu. Select to add a new library to the Global or Project table — select Global and name your library. Once the new library appears in the list, highlight it and then click File and select New Footprint. A dialogue appears and you can name your new footprint: Pim_BMP280_Module.

您还需要点击下拉菜单，指定该元件是SMD（表面贴装）元件还是通孔元件。选择通孔元件，然后添加焊盘和其他封装部分。与PCB编辑器类似，您可以设置网格分辨率。由于BMP280模块的引脚间距为标准的2.54mm，因此建议初始时将网格设置为此值，以便轻松放置引脚。

You also need click the drop-down menu and specify whether this is an SMD or Through Hole component. Select Through Hole, then add the pads and other parts of the footprint. Similar to the PCB Editor, you can set the grid resolution and, as the pins on the BMP280 module are spaced at a standard 2.54mm pitch, it is worth setting the grid to this initially to allow you to easily place the pins.

接下来，点击“添加垫片”工具图标。你需要从左到右依次放置五个编号为 1 到 5 的垫片。最简单的方法是从中心基准线向外数两个网格间距，然后点击放置垫片 1。注意，“添加垫片”工具会递增垫片编号，因此下一个预览的垫片编号为2。将一个垫片移动到你刚刚创建的垫片的右侧，然后再次点击。重复此操作，直到你整齐地排列好五个垫片为止。

Next, click the Add a pad tool icon. You’ll need to end up with five pads labelled 1 to 5 moving from left to right. The easiest way to do this is to count two grid spacings out from the centre datum line and then click to place pad 1. Notice that the Add a pad tool then increments the pad number so the next previewed pad is labelled 2. Move one pad to the right of the pad you just made and click again. Continue until you have a neat row of five pads.

切换回“选择项目”工具，将鼠标悬停在焊盘 1 上，然后按E键打开“焊盘属性”对话框（图 3-6）。在此窗口中，您可以更改焊盘的几何形状、孔径以及更多选项。我们发现，将焊盘尺寸略微增大（高于默认值）并增大孔径，对于在模块之间焊接排针效果很好。您可能有自己的偏好，但我们将每个焊盘都编辑为直径 1.8 毫米、孔径 1 毫米的圆形。

Reverting to the general Select items tool, hover over pad 1 and press the E key to open the Pad Properties dialogue (Figure 3-6). In this window you can change the geometry of the pad, the size of the hole, and many more options. We’ve found that increasing the pad size slightly from the default, and increasing the hole size, works well for soldering header pins between modules. You may have your own preferences, but we edited each pad to be a 1.8mm circle with a 1mm hole.

焊盘制作完成后，下一步需要添加丝印图案，以表示模块实际占用的物理面积。许多元件的数据手册中都会列出封装尺寸，但对于专为原型设计和面包板应用而设计的模块来说，情况并非总是如此。在这种情况下，使用游标卡尺测量封装尺寸将有助于您获得实际尺寸。

With the pads created, you next need to add a silkscreen item that represents the physical area the module will occupy. Many components will have physical package dimensions listed in their datasheet, but that’s not always the case with modules that are really designed for prototyping and breadboard use. In these cases, some investigation with a pair of callipers will help you get the dimensions of the package.

测量 Pimoroni BMP280 后，我们发现引脚焊盘距离边缘 2.54 毫米处为 19 毫米见方的区域，这样可以为模块提供略微偏大的裕量，从而确保安全。选择屏幕右侧的F.Silkscreen图层，然后使用 “绘制矩形”工具绘制并正确放置该区域。

Measuring the Pimoroni BMP280, we realised a 19mm square area with the pin pads 2.54mm from the edge gives a slightly oversized and therefore safe margin for the module. Select the F.Silkscreen layer on the right-hand side of the screen and use the Draw a rectangle tool to draw and position it correctly.

最后，在F.Courtyard图层上添加另一个正方形，使其略微超出刚刚创建的丝网印刷图层正方形的范围。您可以通过将网格间距设置为非常小的值（例如 0.01 毫米），然后在远离丝网印刷矩形的位置绘制一个矩形来实现这一点，以避免网格对齐。

Finally, add another square on the F.Courtyard layer that sits just slightly outside the silkscreen layer square you just created. You can achieve this by setting the grid to a very small spacing value such as 0.01mm and then drawing a rectangle away from the silkscreen rectangle to avoid it snapping.

新建一个边长为 19.4 毫米的正方形，然后可以使用 M 键将其移动到指定位置。这个位于前院层的新正方形为“DRC”（设计规则检查器）提供了一项服务，其边界不应重叠。这意味着，在后续流程中，如果某个元件发生重叠，运行 DRC 时，PCB 上的这条边界将被标记为问题。

Make the new square 19.4mm and then you can use the M key to move the square into position. This new square in the front courtyard layer provides a service called the ‘DRC’ or ‘Design Rules Checker’ with a boundary that shouldn’t be overlapped. This means that later in the process, if a component is overlapping, this boundary on the PCB when you run the DRC will be highlighted as an issue.

板载USB接口

USB On Board

现在您几乎拥有制作 Stamp 和 BMP280 板所需的一切！您可能已经注意到主图中 PCB 板上直接有一个 USB 边缘连接器。这是一种无需添加任何额外元件即可添加 USB 接口的简便方法，不过您需要在该区域（1.6mm 厚的 PCB 板背面）添加大约 1mm 的材料，才能使 USB 连接器能够正确安装。这突出了使用其他已获得适当授权的 KiCad 项目中的库和元件的另一种方法。USB Armory 在其早期 Mk1 版本中就采用了这种 PCB 板边缘 USB 连接器的设计方案。

You’ve now got nearly everything you need to make the Stamp and BMP280 board! You might have noticed a USB edge connector directly on the PCB in the main image. This is a cheap and cheerful approach to adding USB without adding any extra components, although you will need to add around 1mm of material to the back of the 1.6mm thick PCB in this area to actually make the USB connector fit. This highlights another way of using libraries and components from other, suitably licensed, KiCad projects. The USB Armory, which, in an early Mk1 version, used the USB edge connector on PCB approach.

USB Armory 是一个开源项目——您可以从这里下载项目仓库：hsmag.cc/USBArmory。下载完成后，解压缩文件夹，然后使用 KiCad 导航到 hardware 文件夹，标记一，并打开armory.kicad_pro文件。打开后，切换到 PCB 编辑器，选择USB 边缘连接器封装，然后按 E 键。在“封装属性”窗口中，单击“编辑封装”按钮。这应该会在封装编辑器中打开该封装。您可能会收到一条警告，提示该封装是用早期版本的 KiCad 创建的，但保存封装后即可消除此警告。

USB Armory is an open source project — you can download the project repository here: hsmag.cc/USBArmory. Once downloaded, unzip the folder and use KiCad to navigate to the hardware folder, then mark-one, and then open the file armory.kicad_pro. Once open, move to the PCB Editor and select the USB edge connector footprint and press E. In the Footprint Properties window, click the Edit Footprint button. This should open the footprint in the Footprint Editor. You might get a warning that the footprint was made with an earlier version of KiCad, but saving the footprint in the editor should clear this warning.

您应该看到封装焊盘和丝印线（同时也是PCB板边缘切割的参考线）现在已在封装编辑器中打开。编辑器顶部会显示一条警告，提示您当前仅编辑当前项目中的封装。您可以使用“文件”菜单，然后选择“另存为”来重命名此封装并将其保存到您之前创建的自定义库中。由于该库是在全局表中创建的，因此现在可以在任何项目中使用此USB边缘连接器封装。您应该对版本进行一些编辑，更清晰地标记焊盘，然后将其保存到库中。记下每个焊盘的连接方式后，您应该重复之前的步骤，在库中创建一个自定义符号来表示原理图中的USB连接器。

You should see that the footprints pads and the silkscreen line (which doubles as a guide for the edge of the PCB board cut out) are now opened in the Footprint Editor. Across the top of the editor you should see a warning that you are currently only editing the footprint within the current project. You can use File then Save As to rename and save this footprint into your custom library that you created earlier. As that library is created on the Global table, this USB edge connector footprint is now available to use in any project. You should edit your version a little, labelling the pads more clearly, and save it to your library. Making a note of each pad's connectivity, you should repeat the earlier approach to create a custom symbol in the library to represent the USB connector in the schematic.

元件已经创建完成。现在你应该能够像之前一样，将它们放置在原理图中，分配封装，然后导入到PCB中。

That’s the components created. You should now be able to place them in your schematic, assign the footprint and then bring them into a PCB just as you have done previously.

撒网

Casting a net

您可以在图 3-7中看到完整的电路图。在这个电路中，连接点比您之前使用过的要多。虽然您可以像以前那样连接，但结果会非常复杂。为了使电路更清晰易读，您可以使用网络（也称为“网”）。网络是指为每个连接点命名。连接到特定名称网络的每个连接点都被视为彼此连接。

You can see the complete schematic in Figure 3-7. In this circuit, there are more connections than you’ve used previously. While you could wire them up as you did before, the result would be quite a tangled web. To make things a little more readable, you can use networks, aka nets. This is where you give a name to a connection. Every connection to a particularly named net will be considered connected to each other.

要将项目添加到特定网络，您需要添加标签并将其连接到该网络。单击“添加网络标签 (L)”工具图标。然后在原理图中单击，此时将出现“标签属性”对话框。在对话框中，您只需输入网络标签的名称，例如，输入字母“L” A。您可以更改字体和大小，满意后，单击“确定”按钮，即可将A标签放置到原理图中。

To add an item to a particular net, you need to add a label and connect it to this. Click the Add a net label (L) tool icon. You then click in the schematic and the Label Properties dialogue will appear. Into this you simply type the name of your net label, so, for example, type the letter A. You can change the font and size, but when you are happy, click the OK button and you can now place your A label into the schematic.

请注意它有一个小的方形连接器。然后，您可以使用“添加导线”A工具，像连接其他元件一样将导线连接到标签上。您可以使用相同的方法重新创建另一个标签，将其连接到无线连接的另一端，或者您可以复制并粘贴原始网络标签。如果您有更复杂的描述性网络标签名称，最好使用复制粘贴（如果您创建的网络标签拼写错误，它将无法连接，并且您可能需要一段时间才能发现错误）。在这个简单的 H 桥示例中，您实际上不需要使用此技巧，但在下一章中，对于更复杂的设计，使用网络标签确实有助于保持原理图的简洁性和可读性。A

Notice that it has a small square connector. You can then connect a wire to the A label as you would to any other component using the Add a wire tool. You can recreate another A label using the same method to attach to the other end of your wireless connection, or you can copy and paste the original net label. If you have more complex descriptive net label names, it can be a good idea to use copy and paste (if you create a net label with a spelling mistake, it will not connect and may take you a while to discover the error). In this simple H-bridge example, you don’t really need to use this technique but, in the next chapter with a more complex design, using net labels can really help to keep a schematic cleaner and more readable.

将原理图导入PCB时，连接到同一网络的任何线路都会通过杂乱无章的线路连接起来。

When you import the schematic into the PCB, any connections to the same net will be connected by lines in the rats nest.

完成原理图后，就可以将所有内容导入到PCB设计中。但是，在开始放置元件之前，需要先创建电路板轮廓。

Once you’ve made your schematic, you can import everything into a PCB. However, before you get started placing components, you need to create the board outline.

开辟一条道路

Carving a path

要创建电路板轮廓，您无需使用 PCB 编辑器中的图形工具，而是导入在免费开源软件 Inkscape 中绘制的轮廓（图 3-8）。虽然 KiCad 自带的工具非常出色，但在设计图形组件时，Inkscape 也具有一些优势。在本示例项目中，我们在 Inkscape 中绘制了一个简单的电路板轮廓对象，将其保存为 SVG 文件，然后将其导入 KiCad。

To create the board outline, you won’t use the graphical tools in the PCB Editor but, rather, import an outline drawn in the free and open source Inkscape application (Figure 3-8). Whilst the included KiCad tools are excellent, Inkscape can offer some advantages when designing graphic components. For the example project, we drew a simple outline object for the board in Inkscape, saved it as an SVG file, and then imported it into KiCad.

为此，请单击“文件”，然后从下拉菜单中选择“导入”>“图形…” 。在“导入矢量图形文件”对话框中，您可以导航到该文件并选择要导入的工作图层。将图形图层设置为“Edge.Cuts”时，请注意您还可以设置“导入比例”值。在本例中，我们在 Inkscape 中已将电路板轮廓设计为正确的尺寸，因此将导入比例保留为 1.00。但是，如果您要将尺寸过大的图形或徽标（例如 HackSpace 徽标）导入到丝印图层，则此功能非常有用。我们在 Inkscape 中将其反转，然后将其导入到背面的丝印图层。

To do this, click File and then select Import > Graphics… from the drop-down menus. In the Import Vector Graphics File dialogue, you can navigate to the file and select the working layer to import to. Setting the graphic layer as Edge.Cuts, notice that you can also set an Import Scale value. In this instance we designed the board outline to be the correct size in Inkscape, so leave the import scale at 1.00. This function is useful, however, if you have an oversized graphic or logo to import to a silkscreen layer, like the HackSpace logo, we’ve reversed in Inkscape and then imported it onto the back silkscreen layer.

在区域

In the zone

最后，我们在这个电路板上使用的另一种技术是创建与网络标签相连的铜箔覆盖区。这是一种自动连接公共连接组的绝佳方法。例如，许多PCB都会有很多连接到GND网络的连接，因此您可以将一层（或一层的一部分）专门用于此网络，并简单地用铜箔覆盖它（图3-9）。

Finally, another technique that we used on this board is to create flooded copper zones attached to a net label. This is an excellent way of automatically connecting groups of common connections. For example, many PCBs will have lots of connections to the GND net, so you can dedicate one layer (or part of one layer) to this net and simply cover it with copper (Figure 3-9).

您可以创建包含许多不同连接方式的填充区域的复杂系统，但在这个项目中，您只在正面铜箔表面使用了一个填充区域，该区域连接了所有接地焊盘。要实现这一点，在电路板布局完成后，使用“添加填充区域”工具。选择此工具，然后单击以在电路板设计上绘制填充区域，确保您位于正确的图层上。此时将出现一个对话框，您可以从列表中选择网络连接，因此您应该选择GND（图 3-10）。将所有其他设置保留为默认值，在电路板上绘制一个矩形。不必过于担心精度，因为填充区域只会出现在切割边缘的几何形状内。绘制矩形的三个顶点后，您可以右键单击并从下拉菜单中选择“闭合轮廓” 。现在，矩形（或您绘制的其他形状）应该会被填充，您应该可以看到所有先前断开的GND焊盘现在都已连接。

You can create complex systems with lots of different flooded areas with differing connectivity, but in this project you have just used one flood on the front copper surface that connects all pads attached to ground. To do this, once the board is laid out, use the Add a filled zone tool. Select this tool, then click to start drawing a fill area over your board design, ensuring you are on the correct layer. A dialogue appears and you can select the net connection from the list, so you should select GND (Figure 3-10). Leaving all the other settings at the default values, draw a rectangle over the board. Don’t worry too much about accuracy as the flood will only appear inside the edge-cut geometry. Drawing three points of your rectangle you can then right-click and select Close outline from the drop-down menu. The rectangle (or other shape you drew) should now flood, and you should see that all the previously disconnected GND pads are now connected.

虽然填充区域连接了整个GND网络，但您仍然需要手动连接其余部分。在之前的PCB上，由于结构简单，不会出现线路交叉，因此只需使用PCB的一面即可。然而，这次的情况要复杂一些。PCB几乎总是不止一层。对于业余爱好者来说，两层比较常见，但对于复杂的设计，您可以使用四层甚至更多层。默认情况下，PCB编辑器有两层：正面和背面。您可以通过单击右侧窗格中的“B.Cu”来选择背面层。现在，当您绘制线条时，它将位于PCB的背面，并且在PCB编辑器中将显示为不同的颜色（蓝色）。

While the filled zone connects the entire GND net, you still have to wire the rest of it up manually. On the previous PCB, you could get away with just using a single side of the PCB because it was simple enough not to lead to any crossing wires. However, this is a bit more complex. PCBs almost always have more than one layer. Two is common for hobbyists, but you can go to 4 or even more for complex designs. By default, the PCB Editor has two layers, front and back. You can select the back layer by clicking on B.Cu in the right-hand pane. Now, when you draw a line, it will be on the back of the PCB, and will appear in a different colour (blue) in the PCB Editor.

在PCB板的两面都预留导线固然很好，但如何连接这些导线呢？PCB板上的许多元件都是通孔元件，它们可以贯穿整个PCB板，并且可以从两侧连接。你还可以添加“过孔”——这些小孔贯穿并连接PCB板的正反两层。

It’s all well and good having wires on both sides of the PCB, but how do you join them? Many of the components on the PCB are through-hole, and these create a link through the PCB and can be connected on either side. You can also add ‘vias’ — these are small holes that go through and link the front and back layers of the PCB.

要添加过孔，请单击“过孔”工具，然后单击PCB上所需的位置。之后，您可以将导线连接到PCB两侧的过孔上，它们就会连接起来。

To add a via, click on the Vias tool, then click at the place on the PCB where you want it. You can then connect wires to it on either side of the PCB and they’ll be connected.

您可能会发现需要在已填充区域的中心放置轨道。如果遇到这种情况，这不成问题，您只需使用快捷键B重新计算已填充区域，系统就会跳过洪水区域。但这也可能导致系统遗漏已填充区域网络中本应存在的连接；在这种情况下，您可能需要手动连接。

You might find that you need to place a track through the middle of your filled zone. If you do, this isn’t a problem, you just need to use the B hotkey to recalculate the filled zone and it will skip out the area of the flood. It’s possible this will mean that it misses a connection that should be in the net for the filled area; in this case, you may need to connect it in manually.

您可以查看我们最终的项目文件，了解我们如何放置组件和连接线路，但实现方法有很多种，您也可以选择不同的方法。

You can take a look at the finished project file for our solution to placing the components and wiring it up, but there are many ways of doing it and you may choose to do it differently.

精准定位

Precise Placement

PCBA 的最后一步是生成封装位置文件，也称为质心文件。与 BOM 文件类似，它本质上是一个电子表格，其中包含每个放置元件的详细信息，包括坐标和旋转角度。

The final piece of the PCBA puzzle is to generate a footprint position file, also referred to as a centroid file. Like the BOM file, this is essentially a spreadsheet which contains details of each placed component, showing both coordinates and the rotational angle of the part.

要生成此信息，请在 PCB 编辑器中选择“文件”>“制造输出”>“元件布局”。确保您的设置与图 4-6中所示的对话框一致。请注意，如果您的项目包含您希望 JLCPCB 包含的通孔元件，则需要取消选中“仅包含 SMD 封装”选项，并在物料清单 (BOM) 中包含这些通孔元件的 LCSC 编号。

To generate this, in the PCB Editor, select File > Fabrication Outputs > Component Placement. Make sure that your settings match the dialogue box shown in Figure 4-6. Note that if your project contains through-hole components that you want JLCPCB to include, you need to uncheck the Include only SMD footprints option and include the LCSC numbers for those through-hole parts in the BOM.

请勿将之前生成的元件封装 POS 文件或 BOM 文件包含在 Gerber 文件的压缩包中，因为它们需要单独上传。准备就绪后，点击“生成位置文件”按钮。请注意，这将生成两个 POS 文件：一个用于上层，一个用于下层。由于设计是单面的，您只需要上传上层文件即可。

Don’t include this component footprint POS file or the BOM file you generated earlier inside the zip file of Gerbers, as they are uploaded separately. Once you are ready, click the Generate Position File button. Notice that this will generate two POS files: one for the upper layer and one for the lower layer. As the design is single-sided, you are only interested in — and later, only need to upload — the upper layer file.

生成上层 POS 文件后，您需要对电子表格的列标题进行一些修改，才能使其在 JLCPCB 中正常工作。请在电子表格程序中打开生成的文件。您可以使用 LibreOffice Calc、Microsoft Excel 或 Google Docs。

With the upper layer POS file generated, you need to make a few alterations to the spreadsheet column header titles for it to work properly for JLCPCB. Open the file you have generated in your spreadsheet program. You can use LibreOffice Calc, Microsoft Excel, or Google Docs.

接下来，进行以下更改：将第一列的标题“Ref”更改为“Designator”；将“PosX”和“ PosY”分别更改为“Mid X”和“Mid Y”；将“Rot”更改为“Rotation ” ；最后，将“Side”更改为“Layer”（图 4-7）。保存修改后的 POS 文件——现在您已拥有上传到 JLCPCB 服务所需的一切。

Next, make the following changes: change the title of the first column, Ref, to Designator; PosX and PosY to Mid X and Mid Y; Rot to Rotation, and finally, Side to Layer (Figure 4-7). Save the POS file with these alterations — you now have everything you need to upload to the JLCPCB service.

一切准备就绪后，请访问 JLCPCB 网站。点击“标准 PCB/PCBA”选项卡上传 Gerber zip 文件。上传完成后，您应该会在预览窗口中看到电路板正反两面的渲染图（图 4-8）。您可以在此页面上更改电路板类型、材料、厚度等参数。不过，除了将电路板颜色更改为黄色（这纯粹是为了美观——我们想要比标准绿色更亮一些的颜色）之外，我们保留了所有默认设置。

With everything ready, head to the JLCPCB website. Click on the Standard PCB/PCBA tab to upload the Gerber zip file. After a short upload, you should see a render of the upper and lower sides of your board in the preview window (Figure 4-8). You can make changes to the board type, material, thickness, and more on this initial page. However, apart from changing the colour of the board to yellow (this is purely decorative — we wanted something a bit brighter than the standard green), we left everything at the default setting.

在页面底部，您可以点击按钮添加/展开PCBA服务。如图4-9所示，我们选择仅组装顶面（因为元件只位于这一面）。根据您选择的是经济型组装还是标准型组装，您需要选中“边缘导轨/基准标记”或“工具孔”（由JLCPCB添加）选项。这表示对于这些非常小的电路板，JLCPCB服务将创建所需的面板布局。选择所有选项后，点击“下一步”。

At the bottom of the page, you can click a button to add/expand the PCBA services. In Figure 4-9, you can see that we have opted to have the top side assembled only (as you only have components on this side). Depending on whether you’ve selected Economic or Standard Assembly, you’ll want to highlight select either Edge Rails/Fiducials or Tooling holes as Added by JLCPCB option highlighted. This indicates that for these very small boards, JLCPCB services will create any needed panel layouts. With all that selected, click Next.

您将看到由 Gerber 文件上传生成的 PCB 布局的更大预览图。请仔细检查，然后单击“下一步”进入下一个选项卡。预览图将如图4-9所示。单击“添加 BOM 文件”按钮，上传您之前创建的 BOM 文件；然后单击“添加 CPL 文件”按钮，上传您之前创建和编辑的顶层 CSV 位置文件。单击“下一步”，这些文件将被上传和处理，这可能需要几分钟时间，之后您应该会看到电路板和元件布局的渲染图。

You’ll get another larger preview of the PCB layout generated from the Gerber uploads. Check it carefully and then click Next to move to the next tab. This will look like Figure 4-9. Click the Add BOM File button and upload the BOM file you created earlier, then click the Add CPL File button and upload the top layer CSV positional file you made and edited earlier. Clicking Next, these will be uploaded and processed, which may take a few minutes, and you should see a render with the board and the components placed.

让我转圈

Spin me around

通常情况下，此时您会发现元件在封装上的旋转角度不正确。有两种方法可以纠正这个问题。如果您的元件角度是标准的，您可以点击渲染图像中的元件进行高亮显示，然后在高亮显示后，使用 JLCPCB 网页上 PCB 渲染图上方的旋转工具（图 4-10）。您可以反复调整，直到设计看起来正确为止。点击“下一步”将保存这些方向设置，并跳转到“添加到购物车”订购页面。虽然这种方法可行，但另一种选择是打开您创建并上传的位置文件，然后编辑渲染图中显示错误的元件的旋转值。根据我们的经验，两种方法都可以，JLCPCB 的工程师通常会询问元件是否正确放置在封装上（尽管最好不要完全依赖这一点）。

Often, at this point, you will find that components are not rotated correctly on the footprints. There are two ways to correct this, if your components are at standard angles, you can click to highlight a component in the render image and, when they are highlighted, use the rotation tools above the PCB render in the JLCPCB web page (Figure 4-10). You can continue to do this until your design looks correct. Clicking Next will save these orientations and take you to the Add to Basket ordering page. Whilst this is a fine approach, another option is to open the positional file you created and uploaded and then edit the rotational value of the components that have appeared incorrectly in the render. In our experience, either way is fine, and the JLCPCB engineers will usually question if a component isn’t sitting on a footprint correctly (though it’s best not to rely on this).

您只需将订单添加到购物车并付款即可。订单确认付款后，您将定期收到订单列表的更新信息。如果设计较为复杂，建议您在下单后四到六个工作小时登录您的账户，查看订单历史记录详情中关于组件布局的分析。

All that’s left to do is to add the order to your shopping basket and pay. Once the order is confirmed and paid, you get regular updates on the order listing and, if it’s a complex design, it’s worth checking back into your account four to six working hours after placing the order to check the analysis regarding component placing in the order history details.

所有部件都订购完毕后，您只需等待即可。具体时间不固定，但通常很快。我们用 KiCad 设计了这个简单的 H 桥电机驱动器，八天后就拿到了组装好的 PCB 板（图 4-1，本章前面已展示）。

Once everything is ordered, all you have to do is wait. The exact times vary, but it’s often quite quick. We started this simple H-bridge motor driver design in KiCad and had the assembled PCBs (Figure 4-1, shown earlier in this chapter) in our hand eight days later.

提前规划：组件和布局

Planning ahead: components and footprints

在为 JLCPCB 设计电路时，即使在原理图层面，也需要考虑将要使用的元器件及其封装。对于 RP2040 板，我们希望使用表面贴装的 micro USB-B 插座，其中所有 USB 机箱和接地引脚都位于上层——这意味着它可以作为 SMD 元器件进行组装。因此，除了引脚/插座之外，整个单元将由 JLCPCB 完成组装。

When designing for JLCPCB, even at the schematic level, you need to be thinking about what component and footprint you will be using. For the RP2040 board, we wanted to use a surface-mount micro USB-B socket where all the USB chassis and ground points are on the upper layer — this means it could be assembled as an SMD component. As such, apart from the pin headers/sockets, the units would be fully assembled by JLCPCB.

浏览LCSC元件库（lcsc.com）后，我们选择了C132560元件。JLCPCB经常提供EasyEDA的原理图和封装符号。幸运的是，您可以将其导入KiCad（这是KiCad 8的新功能，因此请确保您使用的是最新版本）。

Looking through the LCSC component library (lcsc.com), we opted for the C132560 component. JLCPCB often supplies schematic and footprint symbols for EasyEDA. Fortunately, you can import this into KiCad (this is a new feature in KiCad 8, so make sure you’re running the most up-to-date version).

要获取这些文件，您需要注册一个 EasyEDA 帐户 ( easyeda.com )。在 JLCPCB 库网站的元件页面上，点击 LCSC 元件库中标有“PCB 封装”或“元件符号”的链接，然后在显示元件符号和封装的弹出窗口下方点击“免费试用”按钮。

To get the files, you’ll need to set up an EasyEDA account (easyeda.com). Click the link in the LCSC component library that says PCB Footprint or Symbol on the component page on the JLCPCB library website, then click the Free Trial button underneath the pop-up window that shows the component symbol and footprint.

设置登录后，您应该会看到一个基于浏览器的 EasyEDA 项目，其中只加载了组件的占位图。

After setting up a login, you should see a browser-based EasyEDA project with just the footprint of the component loaded.

EasyEDA 中有多个选项卡，您应该能够找到并切换两个选项卡，一个显示元件原理图符号，另一个显示元件封装。选中元件选项卡并使其显示在视图中后，单击“文件”>“另存为文档”>“另存为（本地）”（图 5-4）。 单击后，应该会下载一个文件类型为 EFOO 的文件。此时，请切换 EasyEDA 中的选项卡，以便查看原理图元件，然后重复相同的“文件”>“另存为文档”>“另存为（本地）”操作，您应该会下载一个文件类型为 ELIBZ 的文件。

There are numerous tabs in EasyEDA and you should be able to find and swap between two tabs, one with the component schematic symbol and one with the component footprint. With the component tab selected and in view, click File > Save As Document Save As (local) (Figure 5-4). When clicked, a file with the filetype EFOO should download. Whilst you are here, swap tabs in EasyEDA so you see the schematic component, then repeat the same File > Save As Document Save As (local) process and you should download a file with the filetype ELIBZ.

在 KiCad 的主项目视图中，单击打开封装编辑器。然后，使用“文件”>“导入”>“封装…”并找到下载的 EFOO 文件（图 5-5）。选择该文件，封装将自动导入。接下来，使用“文件”>“另存为”对话框，以常规方式将封装保存到库或自定义库中。

Moving to KiCad in the main project view, click to open the Footprint Editor. Next, use File > Import > Footprint… and navigate to the downloaded EFOO file, Figure 5-5. Select the file and the footprint will be automatically imported. Next, save the footprint to a library or custom library in the usual way using the File > Save As dialogue.

原理图符号的操作步骤相同。打开符号编辑器，使用导入功能导入您下载的 ELIBZ 文件。如果您是第一次打开符号编辑器或封装编辑器，则需要先选择一个工作库才能导入。不过，您可以将导入的项保存到您选择的任何库中。

The process is the same for schematic symbols. Open the Symbol Editor and use the import function to import your downloaded ELIBZ file. If this is the first time you have opened the Symbol Editor or the Footprint Editor you will need to select a working library before being able to import. However, you can save the imported item to any library you choose.

现在你已经完成了这一步，你可以像使用其他任何符号和封装一样使用该符号和封装。

Now you’ve done this, you can use the symbol and footprint just as any others.

获取 USB 元件符号（及其封装）后，从 KiCad 库中添加RP2040元件。接下来，添加电阻和一对标签，将 D+ 和 D- 连接到 RP2040 上的正确引脚。文档指出，需要创建具有精确尺寸和间距的走线来连接这些线路。为此，请为连接分配一个自定义网络类（net class），这样在 PCB 编辑器中绘制这些走线时，它们就能正确创建。

With the USB symbol (and footprint) sourced, add the RP2040 component from the KiCad library. Next, add resistors and a pair of labels to connect the D+ and D- to the correct pins on RP2040. The documentation states that you need to create the traces for these connections with accurate dimensions and clearances. Do this by assigning a custom net class to the connection, or net, so when you draw these traces in the PCB Editor, they’ll be created correctly.

在原理图编辑器的“原理图设置”对话框中，单击最上方“网络类”窗口中的“+”按钮，添加一个新的网络类并为其命名。请注意，项目中的本地网络类名称应以“/ ”开头——例如，“ /USB_lines” 。选择连接RP2040 D+或D-引脚到您添加的USB_D+或USB_D-标签的线段，然后右键单击。从下拉菜单中选择“分配网络类” 。在“添加网络类分配”对话框中，您应该会看到已选中的标签USB_D+，在其右侧有一个下拉菜单，用于选择网络类——当前为“默认”，但如果您向下滚动，应该可以看到之前添加的USB_lines网络类。选择该网络类，然后关闭对话框。如图 5-6所示，对USB_D-标签重复此操作。

In the Schematic Setup dialogue in the Schematic Editor, click the + button in the uppermost Net Classes window, add a new net class, and give it a name. Note that local net class names within a project should start with a / — use /USB_lines. Select a wire segment that connects the RP2040 D+ or D- pin out to the USB_D+ or USB_D- label that you added, and then right-click. Select Assign Netclass from the drop-down menu. In the Add Netclass Assignment dialogue box, you should see the selected label USB_D+ and, to the right of it, a drop-down menu to select the net class — this is currently Default, but if you click down, you should be able to see the USB_lines net class that you added earlier. Select this, then close the dialogue box. Repeat this for the USB_D- label as shown in Figure 5-6.

打开PCB编辑器后，使用电路板设置工具（位置与原理图设置工具相同）调整网络类变量。这包括走线宽度、走线间距、过孔尺寸等（图5-7）。您需要设置走线宽度和走线间距，以创建USB线路所需的走线——这些关于走线几何形状的信息直接取自RP2040硬件设计 文档（参见2.4.1节， USB）。

After opening the PCB Editor, use the Board Setup tool (in the same positions as the Schematic Setup tool) to adjust the net class variables. This includes the track width, track clearance, via size, and more (Figure 5-7). You’ll need to set the track width and the track clearance to create the track lines that you need for the USB lines — this information on track geometry was taken directly from the Hardware Design with RP2040 documentation (see section 2.4.1, USB).

我们设计了电源稳压器，并找到了一个与最小设计示例类似的器件；然而，JLC 元件C26537多了一个引脚，并且采用的是SOT-223-3封装。我们有匹配的 KiCad 库封装，但为了确保引脚编号正确且匹配，我们还是快速创建了一个自定义原理图符号（图 5-8）。

We laid out the power regulator and found a similar device to the minimal design example; however, the JLC component C26537 had an extra pin and was in the SOT-223-3 package. We have a matching KiCad library footprint, but it was easier to just make a quick custom schematic symbol to ensure that the pin numbering was correct and matching (Figure 5-8).

水晶之谜

Crystal conundrum

在查找最小设计示例项目所使用的元件时，我们遇到的一个难题是晶振；我们在 JLCPCB 元件库中没有找到类似的器件（图 5-9）。我们运用硬件黑客的技巧，研究了其他基于 RP2040 的开源设计所使用的元件，并确保将列表限制在我们已知运行良好的项目中。由于本书前面提到过 Solder Party 的 Stamp，我们查看了它的设计。它看起来简单明了，只用了两个 12pF 的电容，并且在 JLCPCB 上找到了晶振，零件号为C521567。要使用它，需要再次使用 EasyEDA 转换封装。

When looking up the components that the minimal design example project used, one area that challenged us was the crystal; we found no similar device available on the JLCPCB component library (Figure 5-9). Using a consummate hardware hacker’s approach, we looked into what components other open source RP2040-based designs used, making sure to limit the list to projects we knew worked well. Having used Solder Party’s Stamp earlier in this book, we checked out its design. It looked simple and straightforward with just two 12pF capacitors, and on checking JLCPCB, the crystal part was available as part number C521567. To use this, you’d need to again convert the footprint from EasyEDA.

在原理图中布置去耦电容非常简单，您应该利用 KiCad 的文本工具添加注释，以便随时提醒自己重要的信息。例如，在RP2040 的硬件设计文档中，它指出 1uF 电容应该放置在 RP2040 的 44 和 45 引脚附近，因此添加原理图注释作为提醒是很有必要的（图 5-10）。

Laying out the decoupling capacitors in the schematic is straightforward, and you should take advantage of the KiCad text tool to add notes, occasionally acting as reminders for important information. In the Hardware design with RP2040 documentation, for example, it shows that the 1uF capacitors should be placed close to pins 44 and 45 on the RP2040, so it makes sense to add a schematic note as a reminder (Figure 5-10).

最小设计示例中使用的闪存芯片可从 JLCPCB 购买，因此您应该采用相同的设计。在 RP2040 硬件设计 文档中，他们添加了一个可选上拉电阻的封装，但发现对于这款芯片来说并不需要，所以您可以省略这部分设计。闪存芯片及其在 PCB 上的相关走线的关键在于它们都位于连续的接地层之上。这意味着您必须仔细考虑走线布局，尤其是在双层板上，因此请以本项目或 Raspberry Pi 项目作为起点。

The flash memory chip used in the minimal design example is available at JLCPCB and, as such, you should go with the same design. In the Hardware design with RP2040 documentation, they have added a footprint for an optional pull-up resistor but found, with this chip, that it wasn’t needed, so you can omit that part of the design. The important thing about the flash chip and the associated traces on the PCB is that it all sits over a continuous ground plane. This means you must think carefully about routing the traces, especially on a two-layer board, so use this project or the Raspberry Pi project as a starting point.

电路板设计中一个我们尚未探讨的有趣之处在于，它具有多种不同的电压，每种电压都有各自的铜箔覆盖区域。这些区域的制作方法与之前的电路板类似，但需要设置优先级，以便不同的覆盖区域能够独立进行覆盖。因此，在电路板的顶层，有一个通用的 3.3V 覆盖区域，一个连接到VBUS 的覆盖区域（VBUS 是 USB 到稳压器的 5V 输入），以及一个位于 RP2040 封装内的小型 1.1V 区域。如图5-11所示，我们将 1.1V 覆盖区域的优先级设置为 2，VBUS区域的优先级设置为 1，而通用的 3.3V 覆盖区域的优先级设置为 0。这表明它们是相互独立的区域。

One interesting aspect of the board design, that we haven’t looked at yet, is that it has numerous different voltages which each have their own copper flood zones. Making these is like how you make any other copper flood, as in previous boards, but you need to set a priority value so that the different floods know how to flood separately. So, on the top layer of the board there is a general 3V3 flood, a flood connected to the VBUS, which is the 5V input from the USB to the voltage regulator, and there is a small 1V1 zone inside the footprint of the RP2040. Notice in Figure 5-11 that we have assigned the 1V1 flooded area priority 2, the VBUS area priority 1, and the general 3V3 priority 0. This essentially shows that they are separate areas.

我们决定电阻和大部分去耦电容都采用 0402 封装（我们用的是英制尺寸，因为这是业余爱好者中最常用的）。当然，如果我们打算手工组装电路板，就不会选择这种封装，但既然有工程师和机器人来完成这项精细的工作，使用小型封装也无妨。电容值越大，小型封装的电容值精度就越低。因此，虽然 JLCPCB 提供标称 10uF 的 0402 封装元件，但您最好选择更常见、容量更大的 1206 封装。

We decided that for the resistors and most of the decoupling capacitors, we would go for 0402 size packages (we’re using the imperial sizes because these are most common in the hobbyist community). Again, we wouldn’t make this choice if we were planning to assemble this board by hand, but with the assembly engineers and robots doing this fine work, you might as well use the tiny packages. It’s less common for the very tiny packages of capacitor to be of accurate value as they increase in capacitance. So, although JLCPCB does offer components that claim 10uF in 0402 packages, you should go with a more common, larger 1206 variant.

以上涵盖了本项目特有的所有内容。如果您已经完成了前面的章节，可以将之前的经验应用到本项目中。像上一章中的H桥设计这样的小型项目将帮助您熟悉JLCPCB特有的流程。在动手操作RP2040电路板之前，先阅读几遍《RP2040硬件设计》是值得的。最后，请注意，收到组装完成且功能正常的电路板会让人上瘾！

That covers everything unique to this project. If you’ve worked through the previous chapters, you can apply that experience to this project. Smaller projects like the H-Bridge design in the last chapter will help you get used to JLCPCB-specific processes. Reading Hardware design with RP2040 a couple of times before tinkering with an RP2040 board is time well spent. Finally, be warned, having fully assembled and hopefully functional boards delivered to your door is highly addictive!

漫游机器人

Roving Robot

我们将在后续章节的新项目中沿用上一章的RP2040示例。您需要保留原有的RP2040开发板项目，因此需要复制该项目以开发成机器人漫游车平台。

We’re going to use last chapter’s RP2040 example into new projects in future chapters. You’ll want to keep the original RP2040 board project, so you need to make a copy of the project to develop into a robot rover platform.

要复制原始项目，请转到“文件”>“另存为” ，然后选择或创建一个新文件夹来保存项目。在“名称”对话框中输入副本的新名称，然后单击“保存”。虽然并非绝对必要，但最好在文件浏览器中打开新项目文件夹，并删除新项目中不需要的文件。例如，如果您有一个 Gerber 文件文件夹，这些文件可能与新项目无关。任何备份文件也可以删除，因为如果需要，您可能更倾向于返回原始源项目，而不是使用此新分支项目的备份。

To make a copy of the original project, go to File > Save As, then select or create a new folder to save the project to. Type a new name for the copy in the Name dialogue box, then click Save. Although not completely necessary, it’s not a bad idea to then open the new project folder in a file browser and delete any unneeded files for the new project. For example, if you have a Gerber file folder, these probably won’t be relevant to the new project. Any backup files can also be removed as you would probably return to the original source project, if required, rather than use a backup from this new branched project.

第一个新项目是一个轮式机器人。该机器人的基本设计理念是采用四个轮子，全部由N20型电机驱动。这为后续开发提供了多种选择：它既可以使用普通轮子和轮胎，也可以使用麦克纳姆轮——麦克纳姆轮需要单独驱动才能产生其特有的横向和斜向运动。

The first new project is a wheeled robot. The basic premise for the robot is that it is going to have four wheels, all of which are driven by N20-style motors. This gives you options down the line in that it can run with normal style wheels and tyres, but would also work with Mecanum wheels, which need to be driven individually to create the interesting sideways and diagonal motions Mecanum wheels are known for.

设计的一个主要部分是在RP2040板上添加四个电机驱动电路——每个车轮一个。您可以将这四个电机驱动电路添加到A3原理图中，并使用标签或直接接线的方式进行连接。但是，您还可以使用分层图纸来向原理图添加内容。分层图纸是原理图中位于主图纸下方的子图纸，您可以在其中插入可以连接到主顶层原理图的设计。

A primary part of the design is to add four motor driver circuits to the RP2040 board — one for each wheel. You could place the four motor driver circuits into the A3 schematic and wire them using either labels or direct wiring. However, another way you can add content to the schematic is with hierarchical sheets. A hierarchical sheet is a sub-sheet that exists in the schematic below the main page, into which you can insert designs that can be connected to the main top-layer schematic page.

要创建分层图纸，您可以使用原理图编辑器右下角的“添加分层图纸”工具图标，或者按键盘上的S键。接下来，单击并拖动鼠标在原理图中创建一个矩形。单击完成矩形绘制后，将出现“图纸属性”对话框。您可以在此对话框中输入图纸名称，该名称将显示在主原理图页面上的矩形框内。将第一个图纸命名为L9110_Motor_Driver_1。下方有一个用于输入图纸文件名的输入框。目前，该输入框默认显示为untitled.kicad_sch。这是将为该分层图纸创建的单独文件的名称。请将其更改为合适的名称，例如L9110_Motor_Driver_1.kicad_sch。

To create a hierarchical sheet, you can use the Add a hierarchical sheet tool icon found in the lower right-hand area of the Schematic Editor, or you can press the S key on your keyboard. Next, click and drag to create a rectangle in the schematic. When you click to finish the rectangle, the Sheet properties dialogue appears. Into this you can put a sheet name, which will be displayed in the rectangle on the main schematic page. Name the first sheet L9110_Motor_Driver_1. Under this is an input box for a sheet file name. It will currently be populated with untitled.kicad_sch. This is the name of a separate file that will be created for this hierarchical sheet. Change this to something appropriate, such as L9110_Motor_Driver_1.kicad_sch.

请注意，图中标有“显示”的复选框默认处于勾选状态（图 6-4）。这意味着在主原理图中，层级视图矩形将显示，并列出这两项信息。建议显示其中一项或两项信息，否则您必须导航到层级视图才能查看其内容，如果您有多个层级视图，这可能会造成混淆。同样，您还可以调整层级视图矩形的外观，例如增加或减少线宽、背景色和边框颜色。这看似无关紧要，但当您处理包含大量层级视图的设计时，能够通过颜色区分它们可以帮助您更快地完成工作。

Notice that there are checkboxes labelled show and, by default, they will be ticked (Figure 6-4). This means that, in the main schematic sheet, the hierarchical sheet rectangle will appear with both pieces of information listed. It is advisable to show one, or both, of these pieces of information or else you must navigate into the hierarchical sheet to see what it contains, which can be confusing if you have multiple hierarchical sheets. Similarly, notice that you can also play with the appearance of the hierarchical sheet rectangle, increasing or decreasing line width, background, and border colours. This might seem frivolous, but when you work in designs with many of hierarchical sheets, being able to differentiate them by colour can help you work quicker.

要从主原理图页面进入新的层级图纸，您可以右键单击矩形框（图 6-5）并选择“进入图纸”，或者双击层级图纸矩形框。此时应该会看到一个全新的空白原理图。

To enter your new hierarchical sheet from the main schematic page, you can either right-click on the rectangle (Figure 6-5) and select Enter sheet, or you can double-click on the hierarchical sheet rectangle. You should be met with a brand-new empty schematic.

现在您可以开始在层级结构图中放置元件并创建电路。首先需要注意的是，任何连接到全局标签或网络的元件都会自动全局连接到这些点。例如，如果您添加一个元件并将其连接到GND和VCC，它们将自动连接到顶层原理图中的相应点，并且在您将这些元件及其连接导入 PCB 编辑器时也会保持连接状态。

You can now begin to place components and create your circuit in the hierarchical sheet. The first thing to note is that anything connected to a global label or net will automatically be connected to those points globally. If, for example, you add a component and connect it to GND and to VCC, they will automatically be connected to those points in the top-layer schematic and will be connected when you import those components and connectivity to the PCB Editor.

如果您将此类组件放置并连接到分层图纸中，返回主图纸时，您将看不到任何从分层图纸矩形区域引出的连接。对于一般的接地和电源连接，这可能没问题，但如果对所有连接都采用这种方法，则可能会造成混淆。在分层图纸中进行连接的常用方法是使用分层标签。

If you did place and connect such a component in a hierarchical sheet, when you return to the main sheet you won’t see any connections coming out of the hierarchical sheet rectangle. For general ground and power connections this might be OK, but it may get confusing if you use this approach for all your connectivity. A common way of making connections into and out of hierarchical sheets is to use hierarchical labels.

深入挖掘

Digging deep

要添加层级标签，您可以点击“添加层级标签”工具图标，或者按键盘上的 H 键。此时会弹出“层级标签属性”对话框。在“标签”字段中输入名称。现在，您就可以放置、移动、旋转标签，并将其连接到您的设计中。

To place a hierarchical label, you can either click the Add a hierarchical label tool icon or press H on your keyboard. A Hierarchical Label Properties dialogue will appear. Insert a name into the Label field. You will now have a label you can place, move, and rotate and connect into your design.

在图 6-6中，我们创建了层级标签test_hierarchic，并将其连接到 LED 元件符号的阳极端。我们还将全局标签 test 连接到了另一个 LED 元件。退出层级视图非常简单：您可以右键单击并选择“离开视图” ，或者按住ALT键，然后按退格键。

In Figure 6-6, we have made the hierarchical label test_hierarchic and connected it to the anode end of an LED component symbol. We’ve also placed a global label test to another LED component. Moving out of the hierarchical sheet is simple: you can either right-click and select Leave sheet or you can hold ALT and then tap the Backspace key.

即使在层级图纸中创建了层级标签，您也看不到该连接，直到您右键单击层级图纸矩形，然后从下拉菜单中选择“导入图纸引脚”。现在，您应该可以看到所有层级引脚都与矩形边缘对齐。您可以将这些引脚移动到矩形周围的任意位置，并且可以像连接其他符号一样连接和布线这些标签。

Even after creating a hierarchical label inside a hierarchical sheet, you won’t see that connection until you right-click over the hierarchical sheet rectangle and click Import Sheet Pin from the drop-down menu. You should now see any hierarchical pins appear aligned with the edge of the rectangle. You can move these pins to any position around the rectangle, and you can connect and wire to these labels as you would any other symbol.

在图 6-7中，您可以看到图纸矩形内的test_hierarchic标签，它连接到VBUS。请注意，您看不到全局标签test，但该分层图纸内的点将连接到项目原理图中任何带有该全局标签的其他连接。在该分层图纸内，有一个连接到GND符号的连接，因此该点连接到项目的全局GND标签。

In Figure 6-7 you can see the test_hierarchic label in the sheet rectangle, and it is wired to VBUS. Note that you can’t see the global label test, but that point inside the hierarchical sheet will be connected to any other connections with that global label anywhere in the project schematic. Inside this hierarchical sheet, there is a connection to a GND symbol and, as such, that point is connected to the project’s global GND label.

对于机器人漫游车的设计，我们力求简单经济，因此选择了L9110电机驱动IC，因为它适用于N20电机，价格实惠，而且JLCPCB库存充足。L9110周围的电路非常简单（图6-8），电机输出端并联了几个上拉电阻和一个去耦电容。在为电机驱动电路创建层级图时，我们使用层级标签来表示两个信号输入。虽然我们也可以选择将电机输出作为层级标签，但将电机输出连接器符号添加到层级图内部会更简洁，避免主原理图过于杂乱。

For the robot rover design, let’s keep it simple and affordable and use the L9110 motor driver IC as it’s adequate for the N20 motors, affordable, and there is a large amount of stock available on JLCPCB. The circuit around the L9110 is straightforward (Figure 6-8), with a couple of pull-up resistors and a decoupling capacitor across the motor outputs. When we created a hierarchical sheet for the motor driver circuit, we used hierarchical labels to create the two signal inputs. We could have opted to have the motor outputs as hierarchical labels, but it was cleaner to add the motor output connector symbols inside the hierarchical sheet, avoiding more clutter on the main schematic.

使用层级式工作表的一大好处是，您可以快速复制它们（或其内容），从而在同一项目或其他项目中创建多个类似的模块。在机器人漫游车项目中，我们只需添加三个层级式工作表，并按顺序命名为Motor_Channel_1、Motor_Channel_2、Motor_Channel_3和Motor_Channel_4。

One of the great benefits of using hierarchical sheets is that you can quickly copy them (or their contents) to create multiples of similar modules, either within the same project or into other projects. In the robot rover project, we have simply added three more hierarchical sheets and named them sequentially as Motor_Channel_1, Motor_Channel_2, Motor_Channel_3, and Motor_Channel_4.

然后，我们将Motor_Channel_1的内容复制粘贴到各个不同的层级图中。每次复制 L9110 电路时，我们都会重新标记层级引脚，以确保每个电机通道的引脚唯一（图 6-9）。之后，您可以使用之前在每个电机通道层级图中导入引脚的功能，即可将引脚连接到 RP2040 上您选择的 GPIO 引脚——可以直接连接，也可以使用标签连接，以保持主原理图的整洁。

We then copied and pasted the contents of Motor_Channel_1 into each different hierarchical sheet. Each time we copied the L9110 circuit, we relabelled the hierarchical pins so that each motor channel was unique (Figure 6-9). You can then use the Import Sheet Pin function used earlier on each of the motor channel hierarchical sheets, and you are ready to wire the pins to your chosen GPIO pins on the RP2040 — either directly or using labels to again keep the main schematic clean and tidy.

为了帮助你理解层级式图纸，你应该浏览一些使用 KiCad 的开源硬件项目。你肯定会发现许多不同的组织和项目管理方法。

To help you understand hierarchical sheets, you should look through some open-source hardware projects that have used KiCad. You’ll certainly find lots of different approaches to organisation and project management.

摇摇晃晃

Wibbly wobbly

柔性PCB设计在现代电子产品中应用广泛，其中最常见的当属简单的柔性连接器。柔性连接器的优势显而易见，它们可以将系统中不同位置的元件或PCB模块连接起来。柔性连接器可以插入特定的夹紧插座，也可以直接焊接在铜焊盘上。它们能够折叠弯曲，从而实现复杂的PCB布局，而无需使用较大的排针或插座。

Flexible PCB designs are commonplace in modern electronics for many use cases. Probably the most common are simple flex connectors. These have obvious advantages, in that they can connect components or PCB modules in different locations in a system. Flex connectors can be inserted into specific clamping sockets or directly soldered onto copper pads. They have the benefit of being able to fold and bend around, allowing complex layups of PCBs which do not need larger header pins or sockets.

柔性PCB基板种类繁多，最常见的是聚酰胺薄膜。走线和焊盘的工作原理与普通PCB非常相似，都是由一层薄薄的铜构成。柔性PCB的设计可能相当复杂，许多PCB制造商都提供柔性PCB的定制层材料选项。这些柔性PCB也可能包含刚性部分，这意味着您必须提供能够区分不同基板的设计方案。

There are numerous types of flexible PCB substrate, with the most common being polyamide film. Traces and pads work in a very similar manner to any PCB, in that they are a thin layer of copper. Flexible PCBs can become quite complex to design for, and many PCB fabrication houses will have options for custom layer materials in flex PCBs. These can also include rigid sections, which means you must supply a design that can distinguish different substrates within it.

如果您计划使用这项技术，我们建议您阅读PCB制造厂商提供的所有相关指南，并直接与他们沟通，解释您的设计理念。它可能像设计常规PCB一样简单，只需像设计刚性PCB一样导出Gerber文件即可，但也可能存在一些特殊注意事项。

If you plan to use this technology, we’d recommend you read any guidance your PCB fabrication house has and to speak to them directly to explain your concept. It can be as straightforward as laying out a regular PCB design, exporting some Gerbers as you would with a rigid PCB, but there may be specific considerations.

柔性PCB的一个典型应用是柔性天线。我们在网上找到一篇论文，其中包含一张双频2.4GHz和5GHz贴片天线的图片和尺寸，这引起了我们的兴趣，于是我们开始在KiCad中进行布局设计。我们首先在Inkscape中导入了设计所需的PDF源文件，但由于该文件使用了渐变填充，整个对象充满了节点，因此无法正确导出。如果这是一个位图图像，Inkscape的“位图描边”功能就能很好地解决这个问题，但由于它是矢量文件，该功能无法使用。不过，作为矢量图像，我们可以轻松地拖入垂直和水平参考线，并将它们对齐到PDF天线图的边缘（图8-4）。

A good use case for flex PCBs is a flexible antenna. We’d found a paper online with an image and dimensions for a dual-band 2.4GHz and 5GHz patch antenna, which piqued our curiosity, so we set about laying it out in KiCad. We began in Inkscape: we imported the PDF source we had for the design into Inkscape, but it had a gradient fill and therefore wouldn’t export correctly as the whole object was full of nodes. If this was a bitmap image, it would have been a good candidate for Inkscape’s Trace Bitmap function, but as it was a vector file, this wouldn’t work. However, as a vector image, it was straightforward to drag in vertical and horizontal guide lines and snap these to the edges of the PDF antenna drawing (Figure 8-4).

一旦我们有了天线每个部分的参考线，使用钢笔工具围绕该部分绘制连续线，将其闭合形成一个实体对象，就变得很简单了。

Once we had a guide line for every part of the antenna in place, it was a simple job to use the pen tool to draw a continuous line around the part, closing it to form a solid object.

柔性PCB可以弯曲，但多次弯曲后就会开始断裂。具体的断裂频率取决于制造商和具体设计。

Flexible PCBs can be bent, but over multiple bends, they will start to break. Exactly how often will vary between manufacturing houses, and specific designs.

为了延长PCB的使用寿命，在设计柔性PCB时，应避免在走线中使用90度直角，因为PCB弯曲时，这些尖角容易成为撕裂和故障的源头。虽然对于本设计而言，这并非一个主要问题，但我们可以通过选择天线对象，然后使用“路径效果”对话框应用“拐角”路径效果倒角选项（图8-5 ）轻松地为其添加内部和外部径向倒角。最后，我们删除了原始导入的PDF文件，调整文档大小以适应天线设计，然后将其另存为SVG格式。

One thing you can do to prolong the life of the PCB is avoid using sharp 90-degree angles in traces when aiming for a flex PCB as, if the PCB is flexed, the sharp corners can be origin points for tears and failures. Whilst this is not a massive concern for this design, it was easy to add internal and external radial chamfers to the antenna object by selecting the object, then using the Path effects dialogue to apply the Corners path effect chamfer option (Figure 8-5). Finally, we deleted the original imported PDF, resized the document to fit the antenna design, and then saved it as an SVG.

在一个全新的 KiCad 项目中，我们忽略了创建原理图并将元件与原理图符号关联的常规工作流程，直接进入了 PCB 编辑器。无需原理图，即可在 PCB 编辑器中直接添加元件和创建走线。对于更复杂的项目，我们不建议采用这种方法，因为您无法检查连接性或创建网络连接，但对于像这样的小型简单项目来说，这种方法非常便捷。

In a new KiCad project, we ignored the usual workflow of creating a schematic and associating parts to schematic symbols and went straight to the PCB Editor. You can directly add components and create traces in the PCB Editor with no schematic in place. For a more complex project, we wouldn’t recommend this approach, as you have no means of checking connectivity or creating net connections, but for small simple projects like this, it’s easy.

我们导入了天线SVG文件，并确保将其导入到正面铜层（F.Cu）上。然后，我们使用“添加封装”工具添加了两个小型SMD焊盘。我们将这些焊盘放置在原始设计中天线图案的相应位置。由于没有原理图，这些焊盘没有网络连接，它们将直接连接到我们刚刚放置的大型铜天线图案上。当然，这些焊盘上没有阻焊层，因此您可以焊接连接同轴电缆。接下来，只需快速绘制另一个SVG文件作为天线的轮廓，我们使用Inkscape绘制，但您也可以使用KiCad绘制。将轮廓导入到边缘切割层后，您的设计就完成了。

We imported the antenna SVG, making sure to import it onto the Front Copper layer (F.Cu). We then used the Add a Footprint tool to add two small SMD pads. We positioned these on the points in the antenna design that the original design had indicated. With no net connections due to no schematic, these pads will be directly connected to the large copper antenna design that we just placed, but of course, the pads will have no solder mask over them, allowing you to solder on a connecting coaxial cable. All that remains is to then quickly draw another SVG for the outline of the antenna, which we did in Inkscape, but you could just draw in KiCad. With the outline imported to the edge cuts layer, you have a completed design.

为了完成设计制作，我们使用了 OSH Park，他们提供柔性 PCB 板服务。OSH Park 的一个优点是无需生成 Gerber 文件上传——您可以直接将 KiCad PCB 文件上传到网站进行预览和订购。方便的是，项目文件和 Gerber 文件通常不会指定基板或厚度，因此您无需在 KiCad 中指定超薄柔性板设计。但是，如果您需要在宣传中使用 KiCad 设计的渲染图，或者需要将电路板的 3D 模型导出到其他 CAD 程序中使用，那么您可能仍然需要在 KiCad 中精确建模。

To get the design fabricated, we used OSH Park which has a flex PCB offering. One of the nice features of OSH Park is that you don’t have to produce Gerber files to upload — you can upload your KiCad PCB file directly to the website for previewing and ordering. Conveniently, project files and Gerber files don’t particularly specify the board substrate or thickness, so you don’t need to specify a thin flex board design in KiCad. However, you might want to model the board accurately in KiCad, especially if you are using either renders of the KiCad design in promotion or if you are exporting the board 3D model for use in other CAD programs.

您可以使用PCB编辑器中的电路板设置对话框和“物理堆叠”选项卡来模拟柔性电路。您的PCB制造商会提供其柔性PCB产品各层厚度的数据，您可以利用这些数据在电路板设置中设置厚度。如果您只需要一个与您的柔性设计足够接近的PCB视图，您可以简单地调整电路板的主要厚度，方法是将材料更改为聚酰胺，并将该层的厚度设置为0.0102毫米（这是OSH Park柔性聚酰胺层的厚度），如图8-6所示。然后，您可以使用“自定义颜色”选项将顶层和底层阻焊层的颜色设置为透明，方法是将不透明度降低到零。这样，在3D查看器中，您就可以得到一个合理的柔性PCB近似图（图8-7）。

You can use the board setup dialogue and the Physical Stackup tab in the PCB Editor to emulate a flex circuit. Your PCB fabrication house will have data about all the thicknesses of each layer of their flexible PCB offerings and you can use this to set thicknesses in the board setup. If you just need a close enough PCB view that looks like your flex design, you can simply adapt the major thickness of the board by changing the material to Polyamide and setting the thickness of that layer to 0.0102mm (this is the OSH Park flex polyamide layer thickness), as in Figure 8-6. You can then set the colours of the top and bottom solder mask layers to transparent by reducing the opacity to zero using the Custom colour option. This, in the 3D viewer, will then give you a reasonable approximation of a flex PCB (Figure 8-7).

坚如磐石

Hard as nails

通常，PCB制造商会提供用于PCB的金属基板，常见的有铜或铝。当需要快速散热时，这些基板非常有用。例如，对于温度传感器模块，如果既要保证传感器的精度，又不希望电路板吸收过多热量，那么铝基板通常是一个不错的选择。金属基板PCB的另一个应用场景是需要PCB本身作为散热器。例如，我们委托JLCPCB制造并组装了一些1瓦的LED模块（图8-8）。

Often, PCB manufacturers offer metal substrates for PCBs, commonly copper or aluminium. These substrates can be useful when you need to dissipate heat quickly through a system. Often, aluminium substrates can make sense for temperature sensor modules where you want the sensor to be accurate but don’t want the board to soak up heat. Another application for metal substrate PCBs is where you want the PCB to act as a heatsink. For example, we had JLCPCB make and assemble some 1-watt LED modules (Figure 8-8).

这些1瓦的LED灯珠会产生相当多的热量，为了延长其使用寿命，最好配备散热片。LED灯珠背面有一个与电路板连接的大型导热垫，而铝板背面则是裸露的金属。这可以起到LED模块的散热作用，从而降低温度。需要注意的是，铝和铜基板的PCB板在受到压力或负载时可能会弯曲。事实上，当您收到成片的铝基板PCB板时，如果不弯曲PCB板，就很难将其取下。

Running at 1 watt, these LEDs generate a reasonable amount of heat and, to promote their long life, it’s useful to have some kind of heatsink. The reverse side of the LED has a large thermal pad which connects to the board, and the reverse of the aluminium board is bare metal. This acts as a heatsink for the LED module and the temperature is reduced. One thing of note is that aluminium and copper substrate PCBs can be bent if they are put under pressure or load. In fact, when your aluminium PCBs arrive in panels, it can be quite hard to remove them without bending the PCB.

FR4、柔性基板和铝基板并非仅有的选择。对于高速设计、微波频率设计或医疗器械等特殊应用，还有其他基板可供选择，例如罗杰斯基板、聚四氟乙烯基板、特氟龙基板和铜芯基板。这些都是特殊材料，本文不做赘述。

FR4, flexible, and aluminium are not the only options. With high-speed designs, designs running at microwave frequencies, or very special applications like medical devices — there are other substrates available. Rogers, PTFE, Teflon, Copper Core. These are specialist materials, and we won’t look at them here.

规则

Rules Rule

在开发PCB项目时，如果您已选定特定的制造服务商，可以通过设置电路板的设计规则来确保电路板设计的兼容性，使其与该服务商相匹配。设计规则位于我们在第8章“不同基板”中提到的“电路板设置”窗口下，用于设置不同基板的物理叠层特性。

While developing a PCB project, if you have a particular fabrication service in mind, you can ensure your board design’s compatibility by setting up the Design Rules for your board to match the service. The Design Rules is nested under the Board Setup window we used in Chapter 8, Different substrates to set up the different physical stackup characteristics for different substrates.

在PCB编辑器中，导航至“文件”>“电路板设置” ，然后打开名为“设计规则”的下拉菜单。在第一部分“约束”中，您可以设置最小间距、最小走线宽度以及与铜区域相关的其他限制。您还可以调整最小过孔尺寸、孔径和间距，以及丝印层上文本对象的最小尺寸。

In the PCB Editor, navigate to File > Board Setup and then open the drop-down menu labelled Design Rules. In the first section, Constraints, you can set up limits for the minimum clearances, minimum track widths, and other limits relating to the copper regions. You can also adjust the minimum via sizes, hole sizes, and clearances, and the minimum dimensions for text objects on the silkscreen layer.

“设计规则”下拉菜单中的下一个选项是“预定义尺寸”选项卡。本书前面部分已经使用过它来设置项目的走线宽度。不过，需要提醒的是，您可以在项目开始时设置走线宽度，同时考虑目标PCB服务商的任何限制或约束。此外，请注意，您可以从之前的项目中导入设置——如果您要根据特定的PCB服务规范设置项目，这将非常有用。

The next item down in the Design Rules drop-down menu is the Pre-defined Sizes tab. You used this earlier in the book to set track widths for projects. However, as a reminder, you could set this up at the beginning of a project whilst considering any limitations or constraints your target PCB service has. Also, notice that you can import the settings from a previous project — this is helpful if you set up a project for a particular PCB service specification.

跳转到“设计规则”下拉菜单底部，您可以看到“违规严重程度”部分。此部分设置了当项目规则被违反时，设计规则检查器(DRC) 工具的响应方式。首先要提醒的是，在将任何规则设置为“忽略”之前，请务必仔细考虑。虽然对于当前项目而言，您可能并不在意其中的一些问题，但在其他情况下或项目中，被忽略的错误可能会造成严重后果。

Jumping to the bottom of the Design Rules drop-down menu, you can see the Violation Severity section. This section sets up how the Design Rule Checker (DRC) tool responds if any of the rules set for a project are broken. As a primary word of warning, think very carefully before setting any of these to ‘ignore’. It may well be that for a current project you don’t mind some of these issues, but it’s possible under different circumstances or projects, an ignored error could be critical.

返回PCB编辑器窗口，要在项目的任何阶段运行DRC，您可以单击“显示设计规则检查器”窗口工具图标，或者从“检查”下拉菜单中选择“设计规则检查器” 。窗口打开后，您可以单击“运行DRC”按钮，使PCB符合已定义的设计规则。

Back in the PCB Editor window, to run the DRC at any point in your project, you can either click the Show the design rules checker window tool icon or you can select Design Rules Checker from the Inspect drop-down menu. Once the window is open, you can then click the Run DRC button for the PCB to be checked against the defined design rules.

收到错误或警告并不总是意味着您的PCB项目无法正常工作，它们只是表明某些设计规则未得到遵守。规则并非必须遵守，但检查哪些规则被违反始终是有益的，这样可以确保所有违反的规则都是有意为之。例如，在标尺PCB设计中，由于标尺位于切割边缘几何形状的上方，我们遇到了许多丝印错误；此外，由于我们使用的安装孔封装的庭院区域重叠，我们也遇到了许多庭院错误。所有安装孔之间的实际距离都超过了最小间隙，因此这两类问题都无关紧要——尽管如此，检查一下仍然值得。

Getting an error or a warning doesn’t always mean that your PCB project isn’t working, but they are simply indications that there is something that hasn’t met the design rules. Rules don’t always have to be followed, but it’s always good to check which rules are broken so you can be sure that any that are broken are broken intentionally. For example, on the ruler PCB design, we got numerous silkscreen errors as the ruler sat over the edge cut geometry, and we also got lots of courtyard errors where the courtyard areas of the mounting hole footprints we had used had overlapped. All of the actual distances between the mounting holes were over the minimum clearance from each other, so neither of these sets of issues mattered — it was worth checking, though.

运行 DRC 时，会在您的 PCB 设计上添加红色小箭头或标记，突出显示问题所在。即使关闭 DRC 窗口，这些标记仍会保留在您的设计上。在 DRC 窗口关闭的情况下，如果您选择某个标记，该标记所对应的问题将显示在 PCB 编辑器底部的工具栏中。您可以重新打开 DRC 窗口，并使用相应的按钮删除单个或所有标记。当然，如果您不对 PCB 设计进行任何更改就再次运行 DRC，则已删除的标记将被重新添加。

The DRC, when run, will add small red arrows or markers on your PCB design, highlighting where the issues are located. If you close the DRC window, the markers remain on your design. When selecting a marker when the DRC window is closed, the issue that the marker relates to will be shown in the lower toolbar on the PCB Editor. You can reopen the DRC window and delete single markers or all markers using the relative buttons. Obviously, if you don’t make changes to the PCB design and run the DRC again, removed markers will be replaced.

深入探索

Diving deeper

OSH Park 在支持和推广开源项目方面有着卓越的记录，其标志性的紫色阻焊层涂装在众多创客/硬件黑客项目中都非常醒目。然而，OSH Park 经常被推荐为服务商的主要原因之一，或许在于用户可以直接将 KiCad PCB 文件上传到他们的网站——无需再经历创建兼容 Gerber 文件的过程。这使得该服务非常易于使用。如果您是在 KiCad 新版本发布后阅读本文，您可能会发现 OSH Park 网站服务需要一些时间才能完全兼容，但在此期间，您也可以像其他服务商一样上传 Gerber 文件的 zip 压缩包。OSH Park 关于 Gerber 文件设置和要求的指南可在hsmag.cc/Gen_Gerbers上找到。

OSH Park have an excellent track record in supporting and promoting open source projects, and they have an iconic purple solder mask finish which is very visible across lots of maker/hardware hacker projects. However, probably one of the main reasons that OSH Park have often featured as a service is that you can directly upload KiCad PCB files to their website — you don’t have to go through the process of making compatible Gerber files. This makes the service easy to use. If you are reading this after a new milestone version of KiCad has been released, you might find that it takes a little while for the OSH Park website service to become compatible, but you can also upload a zip file of Gerbers in the same way as other services in the interim. OSH Park’s guidance on Gerber set up and requirements is available at hsmag.cc/Gen_Gerbers.

除了标准的 OSH Park 紫色电路板之外，还有 After Dark 版本（黑色基板和透明阻焊层）、更轻的 0.8mm 厚度电路板（配备更厚的 2oz 铜层）以及柔性电路板等选项。虽然它们质量上乘，但对于小型 PCB 设计来说，价格却非常实惠。最后，OSH Park 的沟通服务也十分出色。如果您需要提交工单咨询问题，他们会竭尽全力提供帮助。

Beyond the standard OSH Park purple offering, there are options for the After Dark finish (black substrate and a clear solder mask), a lighter 0.8mm board with a heavier 2oz copper layer, and a flex option. Whilst they offer good quality, they are incredibly affordable when working with smaller PCB designs. Finally on OSH Park, they are excellent at communications. If you need to raise a ticket to ask a question, they go above and beyond.

不同的加工商对您上传的文件及其格式有不同的要求。我们注意到，DRL（钻孔参考线）文件容易出现问题。在 KiCad 中，您可以创建一对 DRL 文件，一个包含未镀通孔，另一个包含镀钻孔；或者您可以将这两个文件合并为一个。JLCPCB 要求这些文件成对提供，而如果您将包含两个独立 DRL 文件的 Gerber 文件上传到 OSH Park，您会收到错误消息，但 OSH Park 会自动在线合并这两个文件并解决问题。

Different fabrication houses have different needs around the files and file formats that you upload. One area we have noticed creating issues is the DRL or drill files. In KiCad, you can create either a pair of DRL files, one containing the non-plated through-holes and another containing the plated drill holes, or you can merge these two files into one. JLCPCB wants these files supplied as a pair, whereas if you upload Gerbers with two separate DRL files to OSH Park, you get an error message, but it conveniently will merge the two files online and solve the issue for you.

有些加工商要求提供钻孔文件，即使PCB设计中并没有钻孔。这在我们第八章“不同基板”中设计柔性PCB天线示例时引发了一个有趣的问题。尽管设计中没有钻孔，我们仍然导出了Gerber文件和DRL文件——这仅仅是因为我们想将Gerber文件上传到不同的服务商处，查看渲染效果并获取报价。

Some fabrication houses want there to be drill files even if the PCB has no drill holes in the design. This caused an interesting issue when we designed the flex PCB antenna example in Chapter 8, Different substrates. We exported the design Gerbers and DRL files even though the design contained no drilled holes — this was just because we wanted to upload the Gerbers to a range of services to see how they rendered and get quotes.

使用 JLCPCB 时，当我们上传柔性天线设计的压缩 Gerber 文件后，预览会忽略边缘切割几何形状（图 9-6），导致设计的圆角错误地消失，电路板显示为直角。与在线客服沟通后，他们确认可以看到边缘切割层，并保证如果我们下单，电路板会正确切割。

With JLCPCB, when we uploaded the zipped Gerber file for the flex antenna design, the preview would ignore the edge cuts geometry (Figure 9-6), so the curved corners of the design would incorrectly disappear, and the board would appear as having square edges. Chatting to the online chat service, they confirmed that they could see the edge cuts layer and assured us that if we placed the order, the board would be cut correctly.

我们尝试调整 Gerber 文件，并在 KiCad 论坛上发帖讨论这个问题。似乎其他人从该项目生成 Gerber 文件后，在 JLCPCB 网站上都能正确渲染。我们发现的区别在于他们没有包含任何钻孔文件。重新上传不带钻孔文件的文件后，电路板的轮廓和边缘切割几何形状都能正确渲染。在此过程中，我们发现 OSH Park 没有这个问题，上传后电路板渲染正常。

We tried playing around with the Gerbers and we also posted the issue on the KiCad forum for discussion. It seemed that others generating their own Gerbers from the project would get a correct render on the JLCPCB site. The difference we spotted was that they weren’t including any drill files. Re-uploading without drill files and the correct board outline and edge cut geometry rendered correctly. As part of this process, we discovered that OSH Park didn’t have this issue and rendered the board correctly at upload.

这个故事告诉我们，Gerber 文件并非标准格式，所以一定要检查你需要什么，如果发现问题，要做好与 PCB 制造商沟通的准备。

The moral of this particular story is that Gerbers aren’t standard, so be sure to check what you need, and be prepared to talk to the PCB manufacturer if things don’t look right.

我们在考察不同的PCB制造服务时，还遇到了与空层相关的另一个问题。将设计上传到PCBWay时，虽然渲染结果正确，但上传过程却会报错，因为铜层的Gerber文件中没有铜（图9-7）。显然，这对于PCB来说非常不寻常，因为铜通常是连接元件和其他部件的导电层。这个标尺项目表明，如果PCB制造工艺更加艺术化，可能会给制造厂带来麻烦。

We had another issue relating to empty layers when looking at different fabrication services. When uploading the design to PCBWay, although it rendered correctly, it would throw an error with the upload because the Gerber file for the copper layers contained no copper (Figure 9-7). Obviously, this is very unusual for a PCB as copper is usually the conductive layer connecting components and more. The ruler project shows that with a more artistic use of PCB fabrication, it’s possible to cause headaches for fabrication houses.

最近我们在向JLCPCB服务部门提交铝基板LED模块项目时遇到了一些问题。我们在JLCPCB元件库中找到的1瓦COB LED，其数据手册上的图示显示，两个半对称的扁平SMD引脚连接器上标有极性标记。我们之前见过这种LED——它们的金属连接器上蚀刻有正负极标记。

We had a problem with a recent project when submitting the aluminium substrate LED module project to JLCPCB services. The 1-watt COB LED we had identified in the JLCPCB parts library had a diagram on the datasheet of the LED which had polarity markings on the two semi-symmetrical flat SMD pin connectors. we’d seen these LEDs in real life — they have an etched - and + in these metal connectors.

当我们将设计稿上传到JLCPCB网站时，网站上渲染的PCB板上元件已正确放置，但JLCPCB提供的LED 3D模型没有极性标记。我们当时认为这样是正确的，而且由于订购数量不多，LED本身体积较大，即使到货后发现极性错误，更换起来也不会太麻烦。下单后，订单流程暂停，JLCPCB联系我们讨论并确认LED的极性。我们不得不指出，这是他们3D模​​型的问题，导致无法判断LED的旋转方向是否正确（图9-8），他们的工程师只有亲自查看包装后才能确定。最终，铝箔LED PCB的生产是正确的。

When we uploaded to JLCPCB, the website rendered the PCB with the components placed and the JLCPCB 3D model of the LED had no polarity markings. we presumed it would be correct, and as only ordering a small number and the LED is a large part, it wouldn’t be too onerous to swap them around if they arrived incorrectly. After ordering, the process was halted, and JLCPCB contacted us to discuss and check the polarity of the LED. We had to point out that it was an issue with their 3D model that meant it was impossible to tell if it was rotated correctly (Figure 9-8), and an engineer at their end would only be able to tell when they physically went and looked at the package. In the end, the aluminium LED PCBs were correctly manufactured.

与任何 PCB 服务商合作的主要经验是，大多数事情都可以通过良好的沟通来实现，而良好的沟通，再加上物理规格，正日益成为选择使用哪家服务商的重要决定因素。

The main takeaway point for working with any PCB service is that most things are achievable with good communication, which increasingly becomes, in combination with the physical specifications, a valuable deciding factor in choosing which service to use.

尺寸增大

Sizing up

Urumbu 社区中已有使用 NEMA 14 电机的案例，这种电机的优点在于通常可以通过 USB 2.0 及以上版本进行控制和供电。然而，大多数小型实验性快速原型机倾向于使用尺寸更大的 NEMA 17 级步进电机。您可以查看任何小型家用或办公用 3D 打印机、小型桌面 CNC 雕刻机或业余绘图仪，都会发现它们使用的是 NEMA 17 电机。

There have been examples in the Urumbu community using NEMA 14 motors, which are convenient in the fact that they can often be controlled and powered by USB 2.0 and above. However, most small experimental rapid prototyping machines tend to use the larger NEMA 17 class of stepper motor. Check out any smaller home- or office-use 3D printer, smaller desktop CNC router, or hobby pen plotter and you’ll find NEMA 17.

以 NEMA 17 为目标，首先需要确定一些机械尺寸并做出一些基本决策。查看 NEMA 17 的数据手册，你会发现封装的外部尺寸为 42 x 42 毫米，并且在 31 毫米见方的四个角上各有一个 M3 螺栓。由于本项目将以最小的 RP2040 电路示例为基础，因此一个好的起点是绘制 NEMA 17 封装图，并将其添加到最小的 RP2040 设计中，以查看其布局效果（图 10-3）。

With NEMA 17 as the target, the first port of call is to find some mechanical dimensions and make some fundamental decisions. Looking at datasheets for NEMA 17, you’ll find that the outer dimensions of the package are 42 by 42mm, and that they have a set of M3 bolts through the assembly in the corners of a 31mm square. Because you’ll use the minimal RP2040 circuit example as the basis of this project, a good starting point is to draw up a NEMA 17 footprint and drop it into the minimal RP2040 design to see how things look (Figure 10-3).

您可以使用 Inkscape 快速绘制 NEMA 17 封装图，然后使用“文件”>“导入”>“图形”将其导入 KiCad 的边缘切割图层。完成此操作后，我们发现需要缩小最小 RP2040 布局中的某些部分尺寸，但缩小幅度并不大，因此您也应该做好相应的准备。您不需要引出所有 GPIO 引脚，这样可以轻松节省空间。电路板上勉强够放一个电机驱动 IC 和外围元件，但最好使用电机驱动模块。这样可以使电路板兼容多种电机驱动器。这意味着您需要在一个轴向上扩展电路板的尺寸。在确定了基本可行性之后，您就可以开始编辑原理图以创建新项目了。

You can draw up a quick NEMA 17 footprint in Inkscape and import it to the edge cuts layer in KiCad using File > Import > Graphics. After we did that, it was obvious that we would have to reduce the size of some aspects of the minimal RP2040 layout, but not unreasonably so you should be prepared to do the same. You won’t need all the GPIO pins broken out, which gives you some easy space-savings. There is just about enough room to also lay a motor driver IC and peripheral components on the board, but you’ll be better off using a module for the motor driver section. This makes the board compatible with a range of motor drivers. This means you need to extend the board dimensions in one axis. With this basic feasibility worked out, you can set about editing the schematic to create the new project.

在原理图编辑器中，删除所有 GPIO 引出接头部分，因为它们不再需要。然后，您可以使用符号编辑器为电机驱动模块创建自定义符号（图 10-4）。创建符号后，使用标签将其连接到 RP2040，以便更清晰地阅读原理图。

In the Schematic Editor, delete all the GPIO breakout header sections as they won’t be needed. You can then use the Symbol Editor to create a custom symbol for the motor driver module (Figure 10-4). With the symbol created, connect it to the RP2040 using labels to keep the general schematic sections easier to read.

使用 NEMA 17 电机而非 NEMA 14 电机的一个区别在于，虽然在一定范围内可以使用大功率 USB 电源以 5V 电压驱动电机，但您可能更希望使用更高的外部电压。大多数常见的步进电机驱动模块都支持此功能，并配有一个“VM”引脚，可用于连接外部电源。

One difference with running a NEMA 17 rather than a NEMA 14 is that although you could, in a slightly limited fashion, run the motor at 5 V from a beefy USB supply, it’s likely you might want to run it from a larger external voltage. Most of the common stepper driver modules can do this and have a ‘VM’ pin into which you can connect an external supply.

为了保留使用 USB 或 VM 的功能，您需要一个外部电源连接器和一个二极管，以便在使用外部电源时保护系统的 USB 端。KiCad 的一大优点是，它采用独立的原理图符号工作流程（然后您可以为每个符号分配元件封装），这意味着您无需立即确定要使用哪个二极管。您可以简单地放置一个二极管符号，将其连接到原理图中，稍后再考虑封装（图 10-5）。

To retain the ability to use either USB or VM, you’ll need a connector for an external supply and a diode to protect the USB side of the system when the external supply is in use. One of the great things about KiCad is that the workflow of separate schematic symbols (to which you then assign a component footprint) means that you don’t have to work out exactly which diode you are going to use right away. You can simply place a diode symbol, wire it into the schematic, and consider the package later (Figure 10-5).

突破

Breaking out

除了电机驱动器之外，您还需要两个连接到 GPIO 和地线的排针插座，以便连接开关作为限位开关；这样，您就可以为使用这些电机开发的任何机器提供反馈和控制选项。同样，您可以直接将这些添加到原理图中。

In addition to the motor driver, you’ll want two header sockets connected to GPIO and ground in case you want to attach switches to act as limit switches; this gives you feedback and control options for any machines that you might develop with these motors. Again, you can simply add these to the schematic.

原理图基本完成后，就可以开始选择元器件，并检查之前使用过的元器件是否仍然有货。在使用PCBA服务时，这一步可能会非常棘手且耗时。截至撰写本文时，我们很高兴地看到JLCPCB仍有RP2040、Winbond闪存芯片和12MHz晶振的库存。我们也花时间确认了电容和电阻等小型元器件也都有库存。

With the adapted schematic largely complete, you can set about making decisions on component choices and check which previously used components are available. This is where things can get very tricky and time-consuming when using PCBA services. At the time of this writing, we were glad to see that the RP2040, the Winbond flash chip, and the 12MHz crystal were still in stock with JLCPCB. We also took the time to check that the smaller components — the capacitors and resistors — were all also in stock.

当时，我们之前使用的USB接口和3.3V稳压器都已缺货。这两款产品周转率都很高，而且在寻找合适的3.3V稳压器的过程中，我们一度找不到任何封装的、适用于本项目的产品。此外，我们还发现，虽然有些稳压器在产品列表中，但无论是产品信息还是元件数据手册，都无法提供足够的信息来决定是否采用该元件。像稳压器这类元件，LCSC（JLCPCB元件仓库的后端供应商）的库存和产品种类都在不断变化和增加。今天在搜索结果中看似棘手的问题，几天后可能就会出现五六个新的选择。

At the time, the USB socket and the 3V3 voltage regulator we had used previously were no longer in stock. Both are high-turnover items and, at one point in this process, we couldn’t identify any 3V3 voltage regulators in any package that were suitable for this project. We also found some challenges in that there would be a regulator listed, but not enough information available either in the listing or the component's datasheet to actually make a decision on whether to include the part. With items like voltage regulators, LCSC (the company that is the back end of the JLCPCB component warehouse) is continually changing and adding items and stock. What can appear a huge problem one day in your search results can suddenly have half a dozen more options in a couple of days' time.

我们最终找到了所有非库存元件的替代品。替换的 USB 接口需要不同的封装，但我们可以从 EasyEDA 下载封装并导入到 KiCad 中（参见“提前规划：元件和封装”）。图 10-6显示了我们找到的新 USB 连接器；我们通过转换产品页面上的 EasyEDA 示例创建了该封装。

We eventually found replacements for all non-stock components. The replacement USB socket required a different footprint, but we could download the footprint from EasyEDA and import it into KiCad (see “Planning ahead: components and footprints”). Figure 10-6 shows the new USB connector we identified; we created the footprint by converting the EasyEDA example on the product page.

新的USB连接器虽然有一些通孔元件，但标签上却标明是SMD（表面贴装）。这让我有些担心，因为PCB组装服务对通孔元件的收费比表面贴装元件高得多，不过最终通过单面表面贴装服务安装时并没有出现问题。

The new USB connector had some through-hole chassis components but was listed as an SMD. This concerned me, as the PCB assembly service charges quite a bit more for through-hole than surface-mount, but the part was attached via the single side surface-mount services without problems.

由于一度找不到合适的电压调节器，我们不得不暂停这个项目两天。后来，我们在JLCPCB元件库中找到了其他库存，并成功找到了一款可以直接替换的SOT23封装的稳压器。务必仔细核对更换元件的封装和引脚排列，确保线路仍然有效。

Having struggled to identify a suitable voltage regulator in any package at one point, we left the project for a couple of days. Later, we found different stock available in the JLCPCB parts library and managed to find a drop-in replacement regulator which would sit on the same SOT23 footprint. It’s definitely worth triple-checking the footprint and pinout of any swapped components to ensure that your wiring still works.

大部分元件问题都已解决，接下来就可以开始编辑PCB布局了。你需要让最小的RP2040布局更加紧凑，以适应NEMA 17封装尺寸，因此应该将RP2040芯片和晶振向上移动，缩短它们与USB接口之间的距离。有时，在重新设计PCB时，抓取功能非常实用。你可以选择一条走线，或者选择一组走线和元件，然后使用G快捷键而不是M键。这样，它不会简单地移动元件，而是会抓取元件，并且走线的连接性保持不变，你可以移动这些元件。根据我们的经验，这种方法很少能得到整齐的走线，但它可以快速创建一个新的布线方案，然后你可以手动编辑它。

With most of the problems solved with regards to components, you can set about editing the PCB layout. You’ll need to make the minimal RP2040 layout more compact to fit within the NEMA 17 footprint, and so you should move the actual RP2040 and crystal upwards, decreasing the distance between it and the USB socket. Sometimes, in reworking a PCB like this, the grab function is quite handy, where you can select a track, or a selection of tracks and components, and then use the G hot key rather than M and, instead of simply moving the objects, they are grabbed and the track connectivity remains which the tracks can move. This rarely results in a neat set of tracks in our experience, but it can be useful to create a quick new routing which you can then manually edit.

PCB设计完成后，下一步是创建项目的Gerber文件、BOM文件和位置文件，并将其上传到JLCPCB。PCB组装完成后，经过短暂的生产和交付，我们使用FreeCAD设计了一个用于3D打印的支架，然后只需使用一些较长的M3螺栓即可将电路板固定到NEMA 17插座上。如果您有兴趣复制这些电路板或尝试RP2040 Urumbu风格的设计，请从书籍库hsmag.cc/kicad_book_files下载此项目。

With the PCB design complete, the next step is to create the Gerbers, BOM, and positional files for the project and upload it to JLCPCB. After a short production and delivery of the assembled PCBs, we created a standoff design for 3D printing using FreeCAD, and then the boards simply attach to a NEMA 17 using some longer M3 bolts. If you are interested in replicating these boards or playing with RP2040 Urumbu-style approaches, download this project from the book repository hsmag.cc/kicad_book_files.

柔和的一面

The softer side

现在电路板已经制作完成，是时候为其编写代码了。您可以使用 Pico SDK 以 C 语言编写代码。您也可以使用 Pico 版本的 MicroPython 或 CircuitPython。但是，由于您创建的是一块新电路板，因此最好为其专门定制固件——即自定义版本的 CircuitPython。这样做的好处有两点：首先，您可以为特定引脚命名，例如，您可以将 GPIO0 替换为 BTN_A；其次，您可以选择要包含的模块。在本项目中，您将添加 Adafruit HID 模块，以便将游戏控制器用作输入设备。

Now that you have created the board, it’s time to write some code for it. You could write the code in C using the Pico SDK. You could also use the Pico build of MicroPython or CircuitPython. However, since you’ve created a new board, it’s helpful to create a firmware tailored specifically for it — a custom build of CircuitPython. This allows you to do a couple of things. Firstly, it lets you name the specific pins, so rather than using, say, GPIO0, you can use BTN_A. Secondly, it lets you select which modules we want to include. In the case of this project, you’ll add Adafruit HID, which enables you to use the game controller as an input device.

我们发现使用适用于 Linux 的 Windows 子系统 (WSL) 构建 CircuitPython 最为简便（图 11-5），但构建 CircuitPython 的一般流程在hsmag.cc/BuildCP 的文档中有所介绍。我们在此不再赘述，请按照该指南设置您的环境。

We found it easiest to build CircuitPython using Windows Subsystem for Linux (Figure 11-5), but the general process for creating a build of CircuitPython is given in the documentation at hsmag.cc/BuildCP. We won’t go through it in detail, so follow that guide to set up your environment.

一切准备就绪后，你需要创建这个开发板。在circuitpython/ports/raspberrypi/boards目录下，将raspberry_pi_pico目录复制到一个新目录中，新目录的名称要与游戏手柄的名称相符。我们将其命名为hackspace_gamepad。

Once you have everything set up, you need to create this board. In the directory circuitpython/ports/raspberrypi/boards, copy the raspberry_pi_pico directory into a new one named appropriately for the gamepad. We called ours hackspace_gamepad.

要为您的开发板定制 CircuitPython，您需要修改两个文件。首先是pins.c 文件，您应该将其编辑为如下所示，这将向 boards 模块添加条目（每个按钮一个条目）：

There are two files that you need to adjust to customise CircuitPython for your board. Firstly, there’s pins.c, which you should edit to read as follows, which adds items to the boards module (one item for each button):

#include "shared-bindings/board/__init__.h"

#include "shared-bindings/board/__init__.h"

STATIC const mp_rom_map_elem_t board_module_globals_table[] = {

STATIC const mp_rom_map_elem_t board_module_globals_table[] = {

    CIRCUITPYTHON_BOARD_DICT_STANDARD_ITEMS

    CIRCUITPYTHON_BOARD_DICT_STANDARD_ITEMS

    { MP_ROM_QSTR(MP_QSTR_UP), MP_ROM_PTR(&pin_GPIO0) },

    { MP_ROM_QSTR(MP_QSTR_UP), MP_ROM_PTR(&pin_GPIO0) },

    { MP_ROM_QSTR(MP_QSTR_RIGHT), MP_ROM_PTR(&pin_GPIO1) },

    { MP_ROM_QSTR(MP_QSTR_RIGHT), MP_ROM_PTR(&pin_GPIO1) },

    { MP_ROM_QSTR(MP_QSTR_LEFT), MP_ROM_PTR(&pin_GPIO2) },

    { MP_ROM_QSTR(MP_QSTR_LEFT), MP_ROM_PTR(&pin_GPIO2) },

    { MP_ROM_QSTR(MP_QSTR_DOWN), MP_ROM_PTR(&pin_GPIO3) },

    { MP_ROM_QSTR(MP_QSTR_DOWN), MP_ROM_PTR(&pin_GPIO3) },

    { MP_ROM_QSTR(MP_QSTR_BTN_A), MP_ROM_PTR(&pin_GPIO18) },

    { MP_ROM_QSTR(MP_QSTR_BTN_A), MP_ROM_PTR(&pin_GPIO18) },

    { MP_ROM_QSTR(MP_QSTR_BTN_B), MP_ROM_PTR(&pin_GPIO19) }

    { MP_ROM_QSTR(MP_QSTR_BTN_B), MP_ROM_PTR(&pin_GPIO19) }

};

};

MP_DEFINE_CONST_DICT(board_module_globals, 

MP_DEFINE_CONST_DICT(board_module_globals, 

                     board_module_globals_table);

                     board_module_globals_table);

接下来，将mpconfigboard.mk文件编辑为以下内容：

Next, edit mpconfigboard.mk to be the following:

USB_VID =0x1209

USB_VID = 0x1209

USB_PID =0xB182

USB_PID = 0xB182

USB_PRODUCT = "HackSpace gamepad"

USB_PRODUCT = "HackSpace gamepad"

USB_MANUFACTURER = "HackSpace magazine"

USB_MANUFACTURER = "HackSpace magazine"

CHIP_VARIANT =RP2040

CHIP_VARIANT = RP2040

CHIP_FAMILY =rp2

CHIP_FAMILY = rp2

EXTERNAL_FLASH_DEVICES = "W25Q128JVxQ"

EXTERNAL_FLASH_DEVICES = "W25Q128JVxQ"

CIRCUITPY__EVE = 1

CIRCUITPY__EVE = 1

FROZEN_MPY_DIRS += $(顶部)/frozen/Adafruit_CircuitPython_HID

FROZEN_MPY_DIRS += $(TOP)/frozen/Adafruit_CircuitPython_HID

在mpconfigboard.mk 文件中，您可以定义闪存芯片的类型，并添加所需的“冻结”模块。冻结模块可以是您希望默认包含在构建过​​程中的任何模块（除了自动包含的核心模块）。冻结模块必须位于circuitpython/frozen目录中，但您应该会发现该Adafruit_CircuitPython_HID模块已经存在于此目录中。

In mpconfigboard.mk, you define the type of flash chip you have and add any ‘frozen’ modules you want. Frozen modules can be anything that you want to be included on the build by default (other than the core modules that are automatically included). Frozen modules must be in the circuitpython/frozen directory, but you should find that the Adafruit_CircuitPython_HID module is already there.

现在，您可以通过访问circuitpython/ports/raspberrypi并运行以下命令来创建您的构建：

You can now create your build by going to circuitpython/ports/raspberrypi and running:

制作 BOARD=hackspace_gamepad

make BOARD=hackspace_gamepad

这将编译你的代码，最终会生成一个名为build-hackspace_gamepad 的目录。在这个目录中，你会找到一个名为firmware.uf2 的文件，你可以像加载其他 UF2 文件一样将其加载到你的游戏手柄上。

This will compile your code, and you should end up with a build-hackspace_gamepad directory. In there, you’ll find a firmware.uf2 file that you can load onto your gamepad just as you would any other UF2 file.

这并非完整的固件——它只是编程语言。现在你需要编写一个程序才能让所有功能正常工作。幸运的是，所有需要的模块都已内置，因此无需安装任何其他模块。以下固件示例借鉴了 CircuitPython 示例代码。将其保存为code.py到设备文件系统的根目录：

This isn’t complete firmware — it’s only the programming language. You now need to write a program to get everything working. Fortunately, you have all the modules we need baked in, so there’s no need to install any additional modules. Here’s some firmware that draws inspiration from the CircuitPython example code. Save it as code.py into the root of the device’s filesystem:

import time

import time

import board

import board

import digitalio

import digitalio

import usb_hid

import usb_hid

from adafruit_hid.keyboard import Keyboard

from adafruit_hid.keyboard import Keyboard

from adafruit_hid.keyboard_layout_us import KeyboardLayoutUS

from adafruit_hid.keyboard_layout_us import KeyboardLayoutUS

from adafruit_hid.keycode import Keycode

from adafruit_hid.keycode import Keycode

# A simple neat keyboard demo in CircuitPython

# A simple neat keyboard demo in CircuitPython

# The pins we'll use, each will have an internal pullup

# The pins we'll use, each will have an internal pullup

keypress_pins = [board.UP, board.DOWN, board.LEFT, 

keypress_pins = [board.UP, board.DOWN, board.LEFT, 

                 board.RIGHT, board.BTN_A, board.BTN_B]

                 board.RIGHT, board.BTN_A, board.BTN_B]

# Our array of key objects

# Our array of key objects

key_pin_array = []

key_pin_array = []

# Keycode sent for each button, will be paired with a control key

# Keycode sent for each button, will be paired with a control key

keys_pressed = [Keycode.UP_ARROW, Keycode.DOWN_ARROW,

keys_pressed = [Keycode.UP_ARROW, Keycode.DOWN_ARROW,

                Keycode.LEFT_ARROW, Keycode.RIGHT_ARROW,

                Keycode.LEFT_ARROW, Keycode.RIGHT_ARROW,

                Keycode.A, Keycode.B]

                Keycode.A, Keycode.B]

# Sleep to avoid a race condition on some systems

# Sleep to avoid a race condition on some systems

time.sleep(1)  

time.sleep(1)  

keyboard = Keyboard(usb_hid.devices)

keyboard = Keyboard(usb_hid.devices)

keyboard_layout = KeyboardLayoutUS(keyboard)  

keyboard_layout = KeyboardLayoutUS(keyboard)  

# Make all pin objects inputs with pullups

# Make all pin objects inputs with pullups

for pin in keypress_pins:

for pin in keypress_pins:

    key_pin = digitalio.DigitalInOut(pin)

    key_pin = digitalio.DigitalInOut(pin)

    key_pin.direction = digitalio.Direction.INPUT

    key_pin.direction = digitalio.Direction.INPUT

    key_pin.pull = digitalio.Pull.UP

    key_pin.pull = digitalio.Pull.UP

    key_pin_array.append(key_pin)

    key_pin_array.append(key_pin)

print("Waiting for key pin...")

print("Waiting for key pin...")

while True:

while True:

    # Check each pin

    # Check each pin

    for key_pin in key_pin_array:

    for key_pin in key_pin_array:

        i = key_pin_array.index(key_pin)

        i = key_pin_array.index(key_pin)

        key = keys_pressed[i]

        key = keys_pressed[i]

        if not key_pin.value:  # Is it grounded?

        if not key_pin.value:  # Is it grounded?

            print("Pin #%d is grounded." % i)

            print("Pin #%d is grounded." % i)

            # "Type" the Keycode or string

            # "Type" the Keycode or string

            keyboard.press(key)  # "Press"...

            keyboard.press(key)  # "Press"...

        else:

        else:

            keyboard.release(key)

            keyboard.release(key)

    time.sleep(0.01)

    time.sleep(0.01)

如您所见，您可以在代码中使用`board.UP`、`board.DOWN`、`board.LEFT`、`board.RIGHT`、`board.BTN_A`和`board.BTN_B`。这有两个优点。首先，它对程序员来说更直观。其次，如果您创建了另一个版本的电路板，按钮位于不同的引脚上，相同的代码仍然可以在两个版本上运行。

As you can see, you can use board.UP, board.DOWN, board.LEFT, board.RIGHT, board.BTN_A, and board.BTN_B in your code. This has a couple of advantages. Firstly, it is more intuitive for programmers. Secondly, if you created another version of the board with the buttons on different pins, the same code could still run on both.

这段代码有点偷懒。例如，按钮没有做防抖处理time.sleep(0.01)。实际上，我们发现这不会造成太多问题，尤其是在某些特定情况下。这意味着它的响应速度不是最快的，所以如果你玩的游戏对响应时间要求很高，比如百分之一秒，你可能需要使用其他方法，例如用 C 语言编写的经过优化的防抖处理。不过，这个控制器本身也不适合这类游戏。此外，它发送的报告数量也相当随意（报告是指从键盘发送到计算机的状态更新）。每次循环会发送六个报告，这意味着每秒发送数百个报告。同样，这不利于性能。但是，它运行稳定可靠，而且易于理解。

This code is a bit lazy. For example, there’s no debouncing on the buttons. In practice, we’ve found that this doesn’t cause many problems, especially with the time.sleep(0.01) in there. This means it’s not the most responsive controller, so if you’re playing games where hundredths of a second matter, you probably want to use something different, such as tuned debouncing written in C. However, this controller isn’t suitable for that type of game anyway. This is also fairly cavalier with the number of reports it sends (a report being a status update sent from keyboard to computer). This will send six of them every loop, which means several hundred a second. Again, this isn’t great for performance. However, it works reliably and is easy to understand.

加载这段代码后，你应该可以将控制器插入任何电脑，电脑都会将其识别为 USB 键盘。按下其中一个按钮，电脑应该会像识别普通键盘一样识别该按键操作。这样，你就可以控制任何需要电脑输入的游戏了。

With this code loaded, you should be able to plug the controller into any computer and it will recognise it as a USB keyboard. Press one of the buttons and the computer should recognise that button press just as it would from any keyboard. With this, you can control any game that takes input from a computer.

创建自定义版本的 CircuitPython 在构建新电路板时并非必要；但是，一旦你经历过这个过程，它就很容易，而且会让你的生活更美好，尤其是在你将电路板分发给其他人时。

Creating a custom version of CircuitPython isn’t essential when you build a new board; however, once you’ve been through the process once, it’s easy, and makes life a little bit nicer, especially if you’re distributing the board to other people.

至此，我们关于 RP2040 的 KiCAD 之旅就结束了。PCB 设计是一个引人入胜且内容丰富的领域，但现在你应该已经掌握了足够的知识来设计与 Raspberry Pi Pico 兼容的电路板，并将其交给 PCB 组装公司进行生产。你应该理解最小设计，并能够根据自身需求进行调整。你可以添加更多硬件，也可以将其精简到最小尺寸。你可以将 PCB 设计成适合项目的特定形状，甚至可以将 PCB 集成到整个结构中。

This concludes our tour of KiCAD with RP2040. PCB design is a fascinating and huge subject, but you should now know enough to design Raspberry Pi Pico-compatible boards, and get them made by a PCB assembly company. You should understand the minimal design and be able to tweak it to your needs. You can add more hardware, or strip it back to its smallest size. You can make the PCB a specific shape to fit in your project, or even make the PCB an integral part of the structure.